[emazed]

hi, i want to run the same simulation for like 10 different velocity and i would like to know if it is possible to run it automatically ?

[vasava]

Couple of ways you can get this done:

1. Parametric setup with workbench. You will have to set up and solve your primary case with workbench. Rest is simple with design point generation. Do refer to fluent and workbench manuals for details.
2. Fluent journal file. Setup your first case and while doing so record a journal file. Edit and use the journal file for other cases. You can combine the journal files to save even more time.

[emazed]

I have already done a parametric setup for some radius and lenght. But can you change the initial inlet velocity in a parametric setup without creating a new case ?
Thank you

[LuckyTran]

A fluent journal file will let you change the inlet velocity with a fixed mesh, i.e. you prepare one case file and run a bunch of simulations with different inlet velocities. However, the journal file executes sequentially so you cannot run 100 simultaneous simulations.

To do geometry change AND velocity changes requires a bit more work, but that was not your question.

The journal file is very simple and nothing to be scared of. It just needs to look something like:

rcd casename
define/boundary-conditions velocity-inlet inletname y y y 10 n 0 y n 1 n 0 n 0 blah blah blah
solve/iterate 10000
wcd casename y
define/boundary-conditions velocity-inlet inletname y y y 12 n 0 y n 1 n 0 n 0 blah blah blah

The difficulty is that the exact stuff you should type in will depend on your case, because you might have different models activated. You should manually go into Fluent and type the define/boundary-conditions stuff into the TUI and write down everything you need to type to complete the blah blah blah part. In this example i read a case and date file called casename and then set the velocity (using magnitude & direction specification) of a surface named inletname. I set the magnitude to 10 m/s, with a constant profiles, in the [1 0 0] direction. Then I tell it to do 10k iterations. Then I save the casename and overwrite the existing file. Then change the inlet velocity magnitude to 12 m/s, and so on.

[vasava]

Originally Posted by emazed

But can you change the initial inlet velocity in a parametric setup without creating a new case ?

Yes, you can. In the velocity setup select New Input Parameter in the drop down menu. Then you can setup Current value for the first case.

Once you do this you should have a design point in the workbench. You will see the inlet velocity for the first case. Here on wards its just as easy as copy-paste.

LuckyTran has already explained usage of journal files.

Addition:
With a quick google search I found this tutorial that is exactly what you are looking for.

[emazed]

Thx a lot i'll try what you both tell me to do.

[FluidWarrior]

Hi,
the most powerful proceed is to use your own scripts, as you can see here, which includes also a Bibliography of useful sites:
https://www.researchgate.net/publica...t_and_ParaVIEW

Have fun!

[pejman_tork]

hi
I want to write a journal file to run in the university supercomputer.I have a few problems with this.
how can i monitor the solution in a journal file ?
and i use udf in my simulation , should i define udf in journal file ?
--------------------------
;fluent simulation input file
;read case file
rc/home/arazpoor/porous/porous.cas
;initialize the solution
solve initialize initialize-flow
;calculation the iteration
solve/set/time-step 300
solve/dual-time-iterate 288 200
;write data file
wd/home/arazpoor/porous.dat
;exit fluent
exit
;confirm exit to prompt
yes
----------------

[FluidWarrior]

Hi,
my first question is about analyzing the solution. What do you want to do? Do you want to store pictures, data...? Do you need to do the analyzing "online" or can you do that afterwards?
I think you should do an "online" analyzing only if you need them for the other simulations.
You can include UDFs and compile them with TUI commands. Have a look at the ANSYS Documentation. The Manual with all commands is called "ANSYS Fluent Text Command List".
You can find the commands here: /define/user-defined/....

A useful link:
compile UDF in journal file

Did this answer your questions?