Table 4.1: Available Command Line Options for Linux and Windows Platforms lists the available command line arguments for Linux and Windows. More detailed descriptions of these options can be found in the following sections.
To obtain information about available startup options, you can type fluent
-help before starting up Fluent.
Table 4.1: Available Command Line Options for Linux and Windows Platforms
| Option | Platform | Description |
|---|---|---|
-act
| all | Load ACT on Fluent startup. |
-aas
| all | Start Fluent in server mode. |
-affinity=x | all | Specifies the process binding (affinity) setting, as described in Parallel Options. |
-cc
| all | Use the classic color scheme. |
-ccp x
| Windows only | Use the Microsoft Job Scheduler where x is the
head node name. |
-cflush
| Linux only | Ensures that the file cache buffers are flushed. |
-cnf=x
| all | Specifies that x is the hosts file or (for
Linux) machine list. |
-gui_machine=<hostname>
| Linux only | Specifies that <hostname> is used for
running Cortex (the process that manages the GUI and graphics). |
-driver
| all | Sets the graphics driver (available drivers vary by platform –
opengl or x11 or
null (Linux) – opengl or
msw or null (Windows)). |
-env
| all | Show environment variables. |
-g
| all | Run without the GUI or graphics. |
-gpgpu=ngpgpus
| Linux and Win64 only | Specifies that ngpgpus GPGPUs per machine should
be used for AMG acceleration. Only available in parallel. |
-gr
| all | Run without graphics. |
-gu
| all | Run without the GUI but with graphics. You cannot interact with the displayed graphics objects. |
-help
| all | Display command line options. |
-hidden
| Windows only | Run in minimized mode. |
-host_ip=host:ip
| Linux only | Specifies that the IP interface host:ip is to
be used by the host. |
-i journal
| all | Reads the specified journal file(s). Read multiple journals at once as
follows: -i example1.jou -i example2.jou -i example3.jou ...
AAS Mode does not support multiple journals from the command
line. |
-lsf | Linux only | Run ANSYS Fluent using LSF. |
-meshing | all | Start Fluent in meshing mode (you must specify Fluent as either 3d or 3ddp). |
-mpi=mpi_name
| all | Specifies that the MPI implementation is
mpi_name. |
-mpiopt="x"
| Linux only | Specifies additional MPI flags (x) to be
included in the run. |
-mpitest
| all | Launches an MPI program to collect network performance data and prints to console (Linux) or to the working directory (Windows). |
-nm
| all | Do not display mesh after reading. |
-pbs | Linux only | Launches ANSYS Fluent under PBS Professional. |
-pcheck | Linux only | Checks all nodes. |
-platform=x | Linux only | Loads a binary that is specially ported for a particular platform, as described in Performance Options. |
-post
| all | Run the ANSYS Fluent postprocessing-only executable. |
-p<ic>
| all | Choose the interconnect <ic>=
default or myr or
ethernet or ib. |
-r
| all | List all releases installed in the current directory. |
-rsh | all | Use rsh for remote connection rather than the default ssh. |
-rsh=<command> | Windows only | Use <command> for remote connection rather
than the default ssh for running on a remote Linux cluster. |
-rx | all | Run release x of ANSYS Fluent. |
-schost=x | all | Specifies that the host machine for system coupling is
x. |
-scid=y | all | Specifies that the session-id for system coupling is
y. |
-sclic=x | all | Specifies that the port and host machine for the system coupling license
is x. |
-scport=y | all | Specifies that the port on the host machine for system coupling is
y. |
-scname=z | all | Specifies that the unique name for a system coupling participant is
z. |
|
|
Linux only | Run ANSYS Fluent under Sun Grid Engine. |
-sgeq queue
| Linux only | Name of the queue for a given computing grid. |
-sgeckpt ckpt_obj
| Linux only | Sets the checkpointing object to ckpt_obj for
SGE. |
-sgepe fluent_pe min_n-max_n
| Linux only | Sets the parallel environment for SGE to
fluent_pe, and specifies that min_n and
max_n are number of min and max nodes requested. |
-stream
| Linux only | Prints the memory bandwidth. |
-tx
| all | Specifies that the number of processors is x.
|
-tmx
| all | Specifies that the number of processors for meshing is
x. |
fluent -act loads ANSYS ACT at Fluent startup. For
additional information about ACT in Fluent, see Customizing Fluent in the Fluent User's Guide.
Note: Fluent automatically selects the best graphics driver for the given runtime
environment, unless you choose a specific graphics driver with the fluent
-driver command line option.
fluent -driver allows you to specify the graphics driver to be
used in the session. For example, on Linux you can specify fluent -driver
opengl, fluent -driver x11, or fluent
-driver null. These options are described in detail in Hiding the Graphics Window Display in the User's Guide. On Windows you can specify fluent -driver
opengl or fluent -driver msw to enable graphics display.
Using msw instead of opengl instructs
ANSYS Fluent to use the Operating Systems Windows driver rather than the hardware
OpenGL driver.
fluent -cc will run Cortex using the classic black
background color in the graphics window.
fluent -gui_machine=<hostname> will run
Cortex on a specified machine (<hostname>). This option is only
available when running on Linux.
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.
fluent -nm will run Cortex without displaying the mesh in
the graphics window.
Important: Download graphics card driver updates directly from the graphics card vendor's website, for example www.nvidia.com. Do not use the "Update Driver" feature offered by the operating system as these can sometimes update to an older version of the driver.
fluent -meshing specifies that Fluent opens in meshing mode
rather than the default solution mode. See the Fluent Meshing User’s Guide 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 in the User's
Guide.
-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) setting,
except when the Microsoft MPI is used in Windows (in that case, the Microsoft MPI affinity
setting is always used); for all other cases, the Fluent affinity setting is used when
x=1, and no process binding is applied when
x=0 (except when the Intel MPI is used on
Windows, in which case the Intel MPI affinity setting is used).
-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 in the User's Guide.
-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 in the User's Guide.
-gpgpu=ngpgpus specifies the number of general purpose graphics
processing units (GPGPUs) per machine to be used for AMG acceleration. For more information,
see Using General Purpose Graphics Processing Units (GPGPUs) With
the Algebraic Multigrid (AMG) Solver in the Fluent User's Guide.
-host_ip=host:ip specifies the IP interface to be used by the
host process (Linux only).
-mpi=mpi_name specifies that mpi_name 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 in the User's Guide.
-pcheck checks the network connections before spawning compute
nodes (Linux only).
-rsh specifies that RSH should be used to spawn remote processes,
instead of the default ssh.
-rsh=<command> specifies that
<command> should be used to spawn remote processes. (Windows
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.)
-tx 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 in the User's Guide.
-tmx 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 -tx.
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 option in the General tab of Fluent Launcher, as described in Starting ANSYS Fluent Using Fluent Launcher.
The -sge option runs ANSYS Fluent under Sun Grid Engine (SGE)
software, and allows you to use the features of this software to manage your distributed
computing resources. Other options that can be employed in conjunction with
-sge are -sgeq queue, -sgeckpt
ckpt_obj, and -sgepe fluent_pe min_n-max_n.
For a detailed explanation of these options, see Part III: Running ANSYS Fluent Under SGE.
The -lsf option allows you to run ANSYS Fluent under
Platform Computing Corporation’s LSF software, and thereby take advantage of the
checkpointing features of that load management tool. For further details about using the
-lsf option, see Part I: Running ANSYS Fluent Under LSF.
Typing fluent version -r, replacing
version with the desired version, will list all releases of the
specified version.
fluent -rx will run release x of
ANSYS Fluent. You may specify a version as well, or you can wait and specify the version when
prompted.
Typing fluent version -env, replacing
version with the desired version, will list all environment variables
before running ANSYS Fluent.
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).
-scid=y (where y is the session-id of
the system coupling run, without quotes) specifies the identity of the coupling service
run.
-sclic=x (where x is the name of the
port and host machine, without quotes) specifies the port and host of the machine with the
system coupling license running (that the co-simulation participant/solver must connect to).
For example, 7468@localhost.
-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 System Coupling Server File (scServer.scs) in the System Coupling 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 in Workbench in the Fluent in Workbench User’s Guide, as well as the System Coupling 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 in the User's Guide, or you can simply type the following command at startup:
fluent [version] [-geometry] [XXxYY+00-50]
where XX and YY are the width and height in pixels, respectively, and +00-50 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.