CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

Parametric analysis in fluent

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Search this Thread Display Modes
Old   September 30, 2005, 22:55
Default Parametric analysis in fluent
Posts: n/a
I want to run a fluent simulation with a physical property (eg. thermal conductivity) that is varying over a range. Is there a way to run multiple simulations by invoking a loop so that different case files are made and corresponding data files are written for this varying physical property in one go! Is there a way for me to not to repeat the same process everytime i change a physical property?
  Reply With Quote

Old   October 3, 2005, 08:46
Default Re: Parametric analysis in fluent
Posts: n/a
If you can figure out the TUI command to change the properties, then you can write a journal file that will do this for you. In the fluent users guide, you can look at the section on running Fluent in batch mode... this will get you started... there's a list of TUI commands, or you can just try things in the fluent window... if you hit return you will get a list of submenus that are available... quick example:

If you hit return one of the menus you will notice is "solve" so type "solve" to see what's available under that... there you'll see "initialize", and under initialize you'll find fmg-initialization... to get to the top menu type "/" (without the " marks). From the top menu (or in your .jou file) you can access fmg initialization using:


Also, any unique character(s) that represents the menu or command you are trying to access can be used... from the top menu, the only submenu that starts with "s" is solve... and within solve, only initialize starts with "i"... so a shorter way of accessing fmg initialization is:

s i fmg

Try things out in the TUI to see if they work... also, some things require responses (like fmg asks if you want to initialize, so the actual command would be "s i fmg yes")

Like I said, try things out in the TUI... anything you can type into the TUI will work in a journal.

Once you have a journal written, you can run it by going to File->Read->Journal

Another option is that after you read your case you can go to File->Write->Journal and Fluent will record the commands you perform to a text file. Then you can open this file and see the commands fluent used... these can be different then the TUI commands though because they are based on the GUI inputs instead.

I think there's a way to write loops using "scheme" language, but I'm not sure how to do it. If there's not too many commands, then you can just copy each setup after the other so it would look something like:

; rc stands for read case rc case1.cas ; it stands for iterate it 1000 ; wd stands for write data (wc would be write case) wd case1.dat (change setting) it 1000 wd case2.dat (change setting) it 1000 wd case3.dat ; exit fluent exit yes

Hope this helps, and good luck, Jason
  Reply With Quote

Old   October 7, 2005, 15:38
Default Re: Parametric analysis in fluent
Posts: n/a
Hi jason, Your advice on running fluent in batch mode really helped. I am trying to figure out on how to invoke a loop using scheme language....but presently I will opt for the simpler method. I will definitely post if i could do anything using scheme. thanks.
  Reply With Quote

Old   October 12, 2005, 13:59
Default Re: Parametric analysis in fluent
Chris Bailey
Posts: n/a
For what it is worth, here's an example of writing a scheme loop. This one will do iterations and generate a few graphs each time it runs (4 times).

Scheme is interesting to learn. It is written mostly using parentheses, which good Scheme programmers ignore. The language was developed to write Fibonnaci sequence generators, but it is unpopular because Scheme textbooks always use Fibonnaci sequence generation as an example, so the only problem it's good for has already been solved.

The loop I mentioned:

(define (iterate_and_graph)

(ti-menu-load-string "/solve/iterate 50 ")

(ti-menu-load-string "/display/close-window 0 ")

(ti-menu-load-string "/display/close-window 1 ")

(ti-menu-load-string "/display/close-window 2 ")

(ti-menu-load-string "/display/close-window 3 ")

(ti-menu-load-string "/display/open-window 0 ")

(ti-menu-load-string "/display/vector velocity pressure , , , , ")

(ti-menu-load-string "/display/open-window 1 ")

(ti-menu-load-string "/display/set/contours/filled-contours? n ")

(ti-menu-load-string "/display/contour stream-function , , ")

(ti-menu-load-string "/display/open-window 2 ")

(ti-menu-load-string "/display/set/contours/filled-contours? y ")

(ti-menu-load-string "/display/contour temperature , , ")

(ti-menu-load-string "/display/open-window 3 ")

(ti-menu-load-string "/display/set/contours/filled-contours? y ")

(ti-menu-load-string "/display/contour mass-imbalance , , ")



(define iterate_graphs

(lambda (n)

(do ((i n (- i 1)))

((zero? i))




(iterate_graphs 4)

  Reply With Quote

Old   November 22, 2010, 05:53
Default hi
New Member
Join Date: Nov 2010
Posts: 9
Rep Power: 15
taherehaghjou is on a distinguished road
I have to do repititive simulation too. Actually I want to find the best solution which fitts the experimental results. Can anybody help me?
taherehaghjou is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
table fan aerodynamic analysis using gambit and fluent ziq FLUENT 24 February 20, 2011 07:31
need help with manifold analysis in fluent anil1886 FLUENT 0 August 29, 2009 10:29
Analysis of 2D airfoils in Fluent Himanshu Main CFD Forum 1 January 11, 2006 16:07
non-dimensional analysis in Fluent Endee FLUENT 8 September 7, 2005 16:16
How does FLUENT fair in absolute heat transfer analysis Steve Aboagye Main CFD Forum 1 August 31, 1998 12:12

All times are GMT -4. The time now is 15:31.