[A]As per ANSYS FLUENT user manual, a dummy two phase flow simulation should be used where the settings remain exactly as per desired two phase flow conditions but volume fraction equation is not solved. Let the simulation progress for enough time steps so that fluid parcel entering the domain can reach outlet. Then turn the volume fraction equation on. The probability of better convergece increases significantly.

[A] Turn OFF secondary gradient on all the cells: (rpsetvar 'temperature/secondary-gradient? #f). By default, this is #t (true). To obtain the value, type: (rpgetvar 'temperature/secondary-gradient?) which will return either #t or #f.

[A]Be informed that "Segmentation Violation" message is not unique to a particular error. There may be many causes to the problems. Following steps can be used to trace them:

• Check the ICEM translation log in its message window. Was the translation clean? If not, rectify them and recheck. If yes, read next point.
• Have you selected the correct option "2D" for 2D mesh?
• Run the utility "Check Mesh" under "Edit Mesh" tab and rectify error messages, if any. Warning messages can be ignored most of the time, to check them.

[A] In most of the cases, the user has to manually set the material for the domain ("fluid" boundary condition) to new material defined.

[A] It requires a small adjustment in Fluent. You have to use TUI: define > boundary-conditions > repair-periodic. Sometimes, creation fails because of slightly non-matching mesh nodes, increasing the matching tolerance up to 0.5 (default is 0.05) may help: grid/modify-zones/match-tolerance.

[A] There are two ways you can accoplish this:

• Write or record a [clean] script [Fluent Journal] for 1st set of simulation. Change only those variables which you want to change. Read it in subsquent case files.
• Once the Case file is set as per your requirements, use TUI "File -> write-BC" to write all the settings to a file. Read it after mesh import in later cases. Change B.C. such as mass flow rate, temperature, etc manually.

 Warning: Thread 62 has 8 contiguous regions.
        creating extn_int1-shadow
        creating extn_int2-shadow 

WARNING: Unassigned interface zone detected for interface 56
WARNING: Unassigned interface zone detected for interface 57
 Checking storage.

Error: Zone interface_bot already in another interface
Error Object: #f

[A]: You need to adjust the size of the window (top-right corner of the "Save Hardcopy" pop-up window).

• For windows, to start Fluent in 3D mode, use "fluent 3d -g -i batch.jou -hidden". Note that without command line option '-hidden', the GUI will still be started but show as an icon. Replace '3d' by '2d' to start fluent in 2-dimensional mode.
• In Windows, a transcript file cannot be generated through command line. It should be (can be) started and stopped withing Fluent session.
• For Linux or Unix environment, the method further depends on shell:
  • For C-shell: fluent 3d -g < Input.jou >& Output.trn &, where Input.jou is journal script to make fluent read all the necessary files and commands and Output.trn is the transcript file which it will write.
  • For Bash (Bourne Shell) and ksh (Korn Shell): fluent 3d -g < Input.jou > Output.trn 2>&1 &
  • Note that the ampersand (&) at the end of the command tells the OS not to wait till completion of the execution of that line. This is also called running the command in background.
• Note the following additional requirement of run Fluent in batch mode:
  • "Confirm file overwrite" should be set to 'Yes' for all batch processing. This is to avoid the user prompt to over-write the case file when save frequency is set.
  • Alternatively, "Hide Questions" and "Exit on Error" can be switched on and let Fluent handle itself
  • Incidentally, all these 3 settings can only be done through GUI and no equivalent script or TUI command is available. Hence, Scheme command, for example (set! *cx-exit-on-error* #t) to switch on "Exit on Error" option, needs to be used.

[A] This can easily be done by starting solver in batch mode. You can prepare many case and data file using Fluent Post and use following input files to keep solver running all the day-and-night. Run Fluent in batch mode and specify following content as Input.jou. Note that the file extension does not need to be .jou, it can be .in as well.

For Linux:
file/read-case-data Case01.cas
solve/iterate 5000
file/confirm-overwrite no
file/write-data Case01.dat
;
file/read-case-data Case02.cas
solve/iterate 5000
file/confirm-overwrite no
file/write-data Case02.dat
;
file/read-case-data Case03.cas
solve/iterate 5000
file/confirm-overwrite no
file/write-data Case03.dat
... so on

call cd .\Case1
call fluent 3d -wait -g -i Case1.jou
call cd ..\Case2
call fluent 3d -wait -g -i Case2.jou

[A]: This message is an indication of TVR exceeding the default limit of 1.0E+5. The primary cause for such an unphysical value may be: Poor mesh quality (i.e., skewness > 0.85 for Quad/Hex, skewness > 0.90 for Tri/Tetrahedral elements). Use of improper turbulent boundary conditions Not supplying good initial values for turbulent quantities.

[A]: Note that all the solvers converted the input "length" dimensions into meter by scaling up/down the input mesh model appropriately. Since, the scaling is usually done about origin of centre of the volume (in 3D) / area (in 2D), the location of point being considered may not be (X0/1000, Y0/1000, Z0/1000). It is always better to find the co-ordinate by mouse-probe function.

• to save and exit, create an empty file named "stop-fluent" in /tmp folder. It will make a "#restart.inp" file in the directory from which batch run was started. The files will be written to the same directory where the original input files were read and will have the same names but with appended current iteration number. By default, the case file will be written
• If the machine has several Fluent sessions running, named check pointing can be used selectively. To stop this particular job, use the following command inside the /tmp directory: "touch exit-fluent-job-1"
• To check your job (i.e. to save data for latest iteration and continue the run) create a file named "check-fluent" in your /tmp directory. Check-pointing code calls the same file I/O routines used by the GUI or TUI and will produce the same error messages if disk space is insufficient In such case, Fluent will not return to the iteration loop.
• To write data file only, execute following Scheme command before iterating: (rpsetvar 'checkpoint/write-case? #f)
• If the machine has several Fluent sessions running, named check pointing can be used to selectively stop a specific Fluent process. A specific check point name can be added to the first line of the batch journal file, as shown below:

(set! checkpoint/exit-filename "/tmp/exit-fluent-job-1")
file/read-case-data sample.cas
solve/iterate 1000
file/write-case-data final.cas

• to save and exit, create an empty file C:\temp\exit-fluent.txt

• This file can contain Scheme commands to execute as well as it can contain other files containing Scheme commands to load
• As per the the standard norm of any operating system and programming language, Fluent will search to locate the Scheme files from the working directory unless full path is specified for each Scheme file in .fluent file.

set! *cx-exit-on-error* #f)
Tturn OFF exit-on-error
(let ((menu (cx-add-menu "USC" #\U)))
(load mysettings.scm)
(load postproc.scm)

[A]: The machine of specified file size may be able to handle such set-up files only for cold flow single phase cases. For energy with radiation models, the memory may fall short. One option is to use single precision as it requires approx. half the memory as compared to double precision. Second option would be to use a cluster for pre-processing and CFD-Post for post-processing (CFD-Post in general is more momory efficient than FLUENT Pre-post.) The TUI command can be generated and tested on a simple problem to avoid run-time errors on cluster. Refer to this page dedicated to scripts, macros and journals.