32.3.1 Starting Parallel ANSYS FLUENT on a Windows System Using Command Line Options

To start the parallel version of ANSYS FLUENT using command line options, you can use the following syntax in a Command Prompt window:

fluent version -t nprocs [-p interconnect ] [-mpi= mpi_type ] -cnf= hosts_file

where

• version must be replaced by the version of ANSYS FLUENT you want to run ( 2d, 3d, 2ddp, or 3ddp).

• -p interconnect (optional) specifies the type of interconnect. The ethernet interconnect is used by default if the option is not explicitly specified. See Table  32.3.1, Table  32.3.2, and Table  32.3.3 for more information.

• -mpi= mpi_type (optional) specifies the type of MPI. If the option is not specified, the default MPI for the given interconnect (HP MPI) will be used (the use of the default MPI is recommended). The available MPIs for Windows are shown in Table  32.3.2.

• -cnf= hosts_file specifies the hosts file, which contains a list of the computers on which you want to run the parallel job. If the hosts file is not located in the folder where you are typing the startup command, you will need to supply the full pathname to the file.

  You can use a plain text editor such as Notepad to create the hosts file. The only restriction on the filename is that there should be no spaces in it. For example, hosts.txt is an acceptable hosts file name, but my hosts.txt is not.

  Your hosts file (e.g., hosts.txt) might contain the following entries:

  computer1
  computer2
  

  The last entry must be followed by a blank line.

  If a computer in the network is a multiprocessor, you can list it more than once. For example, if computer1 has 2 CPUs, then, to take advantage of both CPUs, the hosts.txt file should list computer1 twice:

  computer1
  computer1
  computer2
  

• -t nprocs specifies the number of processes to use. When the -cnf option is present, the hosts_file argument is used to determine which computers to use for the parallel job. For example, if there are 8 computers listed in the hosts file and you want to run a job with 4 processes, set nprocs to 4 (i.e., -t4) and ANSYS FLUENT will use the first 4 machines listed in the hosts file. Note that this does not apply to the Compute Cluster Server (CCS).

For example, the full command line to start a 3d parallel job on the first 4 computers listed in a hosts file called hosts.txt is as follows:

fluent 3d -t4 -cnf=hosts.txt

As another example, the full command line to start a 3d symmetrical multiprocessing (SMP) parallel job on 4 computers is as follows:

fluent 3d -t4

In either case, the default interconnect ( ethernet) and the default communication library ( HP-MPI) will be used since these options are not specified.

The first time that you try to run ANSYS FLUENT in parallel, you will be prompted for information about the current Windows account. For more information, see the HP-MPI setup FAQ in the Frequently Asked Questions section of the User Services Center.

The supported interconnects for dedicated parallel ntx86 and win64 Windows machines, the associated MPIs for them, and the corresponding syntax are listed in Tables  32.3.1- 32.3.3:

Table 32.3.1: Supported Interconnects for the Windows Platform

Platform	Processor	Architecture	Interconnects*
Windows	32-bit 64-bit	ntx86 win64	ethernet (default) ethernet (default), infiniband, myrinet

(*) Node processes on the same machine communicate by shared memory.

Table 32.3.2: Available MPIs for Windows Platforms

MPI	Syntax (flag)	Communication Library	Notes
hp	-mpi=hp	HP-MPI	(1), (2), (3)
ms	-mpi=ms	Microsoft MPI	(1), (2), (3)
mpich2	-mpi=mpich2	MPICH2 MPI	(1), (2)

(1) Used with Shared Memory Machine (SHM) where the memory is shared between the processors on a single machine.
(2) Used with Distributed Memory Machine (DMM) where each processor has it's own memory associated with it.
(3) Used with the job scheduler. See Section  32.3.1 for more information.

Table 32.3.3: Supported MPIs for Windows Architectures (Per Interconnect)

Architecture	Ethernet	Myrinet	Infiniband
ntx86	hp (default), mpich2	-	-
win64	hp (default), mpich2, ms	ms	ms

Starting Parallel ANSYS FLUENT with the Microsoft Job Scheduler

The Microsoft Job Scheduler allows you to manage multiple jobs and tasks, allocate computer resources, send tasks to compute nodes, and monitor jobs, tasks, and compute nodes.

ANSYS FLUENT currently supports Windows XP, Vista, as well as the Windows Server operating systems. The Windows Server operating systems include a "compute cluster server" (CCS) and a high performance computing server (HPC) that combines the Microsoft MPI type ( msmpi) or the HP-MPI type ( hpmpi) and the Microsoft Job Scheduler. ANSYS FLUENT provides a means of using the Microsoft Job Scheduler using the following flag in the parallel command:

-ccp head-node-name

where -ccp indicates the use of the compute cluster server package, and head-node-name indicates the name of the head node of the computer cluster.

For example, if you want to use the Microsoft Job Scheduler to run a 3D model on 2 nodes, the corresponding command syntax would be:

fluent 3d -t2 -ccp head-node-name

The first time that you try to run ANSYS FLUENT in parallel for HP-MPI, you need to set the HP-MPI password, either through the Cache HP-MPI Password option in FLUENT Launcher (see Section  32.2), or through the -cache_password command line option (e.g., fluent 3d -t2 -cache_password -cnf=host.txt). After you have set the option, or have issued the command, a dialog prompts you to cache the password or not. Click Yes, then enter the password in the Command Window. Once the username and password have been verified and encrypted into the Windows Registry, then parallel ANSYS FLUENT will launch.

By default, ANSYS FLUENT will run using msmpi. If you want to specify HP-MPI with the Microsoft Job Scheduler, then you can use the following syntax:

fluent 3d -t2 -mpi=hp -ccp head-node-name

Though the usage described previously is recommended as an initial starting point for running ANSYS FLUENT with the Microsoft Job Scheduler, there are further options provided to meet your specific needs. ANSYS FLUENT allows you to do any of the following with the Microsoft Job Scheduler:

• Request resources from the Microsoft Job Scheduler first, before you launch ANSYS FLUENT.

  This is done by first submitting a job that will run until canceled, as shown in the following example:

  job new /scheduler: head-node-name /numprocessors:2 /rununtilcanceled:true

  This example requests a 2-node resource on a cluster named head-node-name. You will see that a job is created with the job ID job-id:

  job submit /scheduler: head-node-name /id: job-id

  Then check if the resources have been allocated:

  job view job-id /scheduler: head-node-name

  If the resources are ready, you can start ANSYS FLUENT using the job ID:

  fluent 3d -t2 -ccp head-node-name -jobid= job-id

  This job will be reusable until you decide to cancel it, at which point you must enter the following:

  job cancel job-id /scheduler: head-node-name

• Have ANSYS FLUENT submit a CCS job, but delay the launching of ANSYS FLUENT until the actual resources are allocated.

  This is done by specifying the job ID as -1, as shown in the following example:

  fluent 3d -t2 -ccp head-node-name -jobid=-1

  If you want to stop the job application, click the Cancel button. ANSYS FLUENT will prompt you for confirmation, and then clean up the pending job and exit.

• Run your job using XML template files.

  This is done by first creating an XML template file, such as shown in the following example:

  <?xml version="1.0" encoding="utf-8"?>
  <Job
     xmlns:xsi="http://www.w3.org/2001/XMLSchema-instance"
     xmlns:xsd="http://www.w3.org/2001/XMLSchema"
     SoftwareLicense=""
     MaximumNumberOfProcessors="4"
     MinimumNumberOfProcessors="4"
     Runtime="Infinite"
     IsExclusive="true"
     Priority="Normal"
     Name="Name_of_job"
     Project="Fluent runs"
     RunUntilCanceled="false">
   <Tasks xmlns="http://www.microsoft.com/ComputeCluster/">
     <Task
         MaximumNumberOfProcessors="4"
         MinimumNumberOfProcessors="4"
         Depend=""
         WorkDirectory="\\file-server\home\user"
         Stdout="fluent-case.%CCP_JOBID%.out"
         Stderr="fluent-case.%CCP_JOBID%.err"
         Name="My Task"
         CommandLine="\\head-node\fluent-sharename\win64\fluent.exe 3d -i bsi.jou -t4"
         IsExclusive="true"
         IsRerunnable="false"
         Runtime="Infinite">
     </Task>
   </Tasks>
  </Job>
  

  where fluent-sharename is the name of the shared directory pointing to where ANSYS FLUENT is installed (e.g., C:\Program Files\ANSYS Inc\v120\fluent).

  Note that you must create a journal file that exits ANSYS FLUENT at the end of the run, and refer to it using the -i flag in your XML template file ( bs1.jou in the previous example).

  After you have saved the file and given it a name (e.g., job1.xml), you can submit the job as shown:

  job submit /jobfile:job1.xml

• Run the job in batch mode without displaying the ANSYS FLUENT GUI.

  The following is an example of such a batch mode job:

  job submit /scheduler: head-node-name /numprocessors:2 /workdir:\\file-server\home\user \\head-node\fluent-sharename\ntbin\win64\fluent.exe 3d -t2 -i bs1.jou where fluent-sharename is the name of the shared directory pointing to where ANSYS FLUENT is installed (e.g., C:\Program Files\ANSYS Inc\v120\fluent).

  Note that you must create a journal file that exits ANSYS FLUENT at the end of the run, and refer to it using the -i flag in your batch mode job submission ( bs1.jou in the previous example).

You can start ANSYS FLUENT jobs from any machine on which is installed either the full CCP or the CCP client tools, but note that all the machines must have the same version installed.