To run Ansys Fluent in the background in a C-shell (csh) on a Linux system, type a command of the following form at the system-level prompt:

fluent 2d -g < inputfile > & outputfile & 

or in a Bourne/Korn-shell, type:

fluent 2d -g < inputfile > outputfile 2>&1 & 

In these examples,

The file inputfile can be a journal file created in an earlier Ansys Fluent session, or it can be a file that you have created using a text editor. In either case, the file must consist only of text interface commands (since the GUI is disabled during batch execution). A typical inputfile is shown below:

 ; Read case file 
 rc example.cas
 ; Initialize the solution
 /solve/initialize/initialize-flow
 ; Calculate 50 iterations 
 it 50
 ; Write data file 
 wd example50.dat
 ; Calculate another 50 iterations 
 it 50
 ; Write another data file 
 wd example100.dat
 ; Exit Fluent 
 exit 
 yes 

This example file reads a case file example.cas, initializes the solution, and performs 100 iterations in two groups of 50, saving a new data file after each 50 iterations. The final line of the file terminates the session. Note that the example input file makes use of the standard aliases for reading and writing case and data files and for iterating. (it is the alias for /solve/iterate, rc is the alias for /file/read-case, wd is the alias for /file/write-data, etc.) These predefined aliases allow you to execute commonly used commands without entering the text menu in which they are found. In general, Ansys Fluent assumes that input beginning with a / starts in the top-level text menu, so if you use any text commands for which aliases do not exist, you must be sure to type in the complete name of the command (for example, /solve/initialize/initialize-flow). Note also that you can include comments in the file. As in the example above, comment lines must begin with a ; (semicolon).

An alternate strategy for submitting your batch run, as follows, has the advantage that the outputfile will contain a record of the commands in the inputfile. In this approach, you would submit the batch job in a C-shell using:

fluent 2d -g -i inputfile  >& outputfile & 

or in a Bourne/Korn-shell using:

fluent 2d -g -i inputfile > outputfile 2>&1 & 

To run Ansys Fluent in the background on a Windows system, the following commands can be used:

fluent 3d -g -i journal 

fluent 3d -g -wait -i journal 

fluent 3d -hidden -i journal 

In these examples,

To get an output (or transcript) file while running Ansys Fluent in the background on a Windows system, the journal file must contain the following command to write a transcript file:

; start transcript file
 /file/start-transcript outputfile.trn 

where the outputfile is a file that the background job will create, which will contain the output that Ansys Fluent would normally print to the screen (for example, the menu prompts and residual reports).

See Creating and Reading Journal Files for details about journal files. See Creating Transcript Files for details about transcript files.

During a typical session, Ansys Fluent may require feedback from you in the event of a problem it encounters. Ansys Fluent usually communicates problems or questions through the use of Error dialog boxes, Warning dialog boxes, or Question dialog boxes. While executing Ansys Fluent in batch mode, you may want to suppress this type of interaction in order to, for example, create journal files more easily.

There are three common batch configuration options available to you when running Ansys Fluent in batch mode. You can access these options using the Batch Options dialog box (Figure 4.6: The Batch Options Dialog Box).

 File → Batch Options...

Figure 4.6: The Batch Options Dialog Box

The Batch Options dialog box contains the following items:

file → set-batch-options

Any combination of these options can be turned on or off at any given time prior to running in batch mode.