CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Fluent Batch Mode - TUI

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

Like Tree1Likes
  • 1 Post By kad

Reply
 
LinkBack Thread Tools Display Modes
Old   July 23, 2012, 16:30
Smile Fluent Batch Mode - TUI
  #1
New Member
 
Diane
Join Date: Jul 2012
Posts: 3
Rep Power: 5
Diane is on a distinguished road
Hello,

I'm new to using the TUI in Fluent. I am trying to set up a batch to run multiple cases where it will pull the data I am interested in for each case before proceeding to the next case (x velocity, surface heat transfer coeff., etc.). I am interested in writing xy data to a file for particular walls and line/rakes (this is for a 2D analysis).

I have looked through the text command list PDF, but the ones that seemed to make sense gave me errors or empty files. Is there a trick to this? Any help/hints you may have would be most appreciated. I'm using Ansys Fluent 13.0.

Thanks,
Diane
Diane is offline   Reply With Quote

Old   July 24, 2012, 02:56
Default
  #2
Senior Member
 
Marion
Join Date: Jul 2012
Location: France
Posts: 122
Rep Power: 6
Marion is on a distinguished road
Hi,
Can you post a copy of the script you are using here? It would be easier to see if there are errors.
Marion.
Marion is offline   Reply With Quote

Old   August 2, 2012, 15:42
Default
  #3
New Member
 
Diane
Join Date: Jul 2012
Posts: 3
Rep Power: 5
Diane is on a distinguished road
Right now the only thing I have gotten to work is to read in a .cas file that has already been set up, iterate, and then write a .dat file:

rc StraightCircleRamp_1200G_20_90deg.cas.gz
/solve/initialize/initialize-flow
it 100000
wd StraightCircleRamp_1200G_20_90deg.dat.gz
rc StraightCircleRamp_1200G_20_3deg.cas.gz
/solve/initialize/initialize-flow
it 100000
wd StraightCircleRamp_1200G_20_3deg.dat.gz
rc StraightCircleRamp_1200G_20_5deg.cas.gz
/solve/initialize/initialize-flow
it 100000
wd StraightCircleRamp_1200G_20_5deg.dat.gz
exit
yes

If you know how to write xy plot data to a file, that would be wonderful. Also, I have noticed that while if it converges, it will continue on to the next simulation, if it diverges and causes the simulation to error out, the entire batch stops. Is there a way to not have that happen?

Thanks,
Diane
Diane is offline   Reply With Quote

Old   August 3, 2012, 03:47
Default
  #4
Senior Member
 
Marion
Join Date: Jul 2012
Location: France
Posts: 122
Rep Power: 6
Marion is on a distinguished road
Hi Diane,
If there is a way to prevent the batch from stopping when something goes wrong I do not know it...
I did some xy plot writing using the TUI a while ago, but it was with an older version of Fluent. I'll have a look on V13 and try to write it again.
Marion.
Marion is offline   Reply With Quote

Old   August 3, 2012, 04:37
Default
  #5
Senior Member
 
Marion
Join Date: Jul 2012
Location: France
Posts: 122
Rep Power: 6
Marion is on a distinguished road
Diane,
Here are the commands for plotting velocity vs. X axis coord on a line (here "line-11" - surface n.11). the xy file is called "titi.xy"

plot
plot
yes
titi.xy
no
no
no
mixture (I am running the mixture model -- you may not need this line)
velocity
yes
1
0
0
line-11
()

when you type it in Fluent 13 here is what you get:
/plot> plot
node values? [yes] y
filename [""] yoo.xy
order points? [no] n
Y Axis direction vector? [no]
Y Axis curve length? [no]

of domain> mixture
cell function> velocity
X Axis direction vector? [no] y
ix [1]
iy [0]
iz [0]
(11)
surface id/name(1) [11] line-11
surface id/name(2) [()] ()

The easiest way to write TUI command lins is to type it directly into Fluent - that's what I just did.
I hope this helps,
Marion.
Marion is offline   Reply With Quote

Old   August 6, 2012, 00:20
Default
  #6
New Member
 
Ganapathy Iyer
Join Date: Mar 2009
Location: Pune, Maharashtra, India
Posts: 25
Rep Power: 8
Ganapathy is on a distinguished road
Whenever I do this, I use a batch file (in windows) or a shell script to do this. I fire fluent with a corresponding script file i.e. fluent 3d -i new.jou
In this way, if one of the cases gets screwed, the others still fire
Ganapathy is offline   Reply With Quote

Old   August 6, 2012, 03:58
Default
  #7
Member
 
Touré
Join Date: Aug 2010
Location: Montréal
Posts: 85
Rep Power: 6
Touré is on a distinguished road
As Ganapathy has said, a good practice is to use a journal file.
To run you journal file:
1. Open a DOS command window (cmd.exe)
2. Type
dir C:\Users\Diane\Desktop\Test_blablabla\

3. Type

"C:\Program Files\ANSYS Inc\v130\fluent\ntbin\win64\fluent.exe" 2ddp -t2 -hidden -i C:\Users\Diane\Desktop\Test_blablabla\fluent_case. jou > outpout.txt

2ddp for 2D (2d) problem and double precision (dp)
t2 for parallel computing on 2 cores
hidden for batch mode
-i something for what I don't remember
fluent_case.jou is your jour nal fil where you copy all your code line (rc .... ............... wd ......)
output.txt for the summarizing of what happened during the simulation like crashing stuff
Touré is offline   Reply With Quote

Old   November 28, 2012, 10:25
Default
  #8
vix
New Member
 
Vikram M.
Join Date: Jan 2011
Posts: 8
Rep Power: 6
vix is on a distinguished road
Hi guys,

I am also looking to queue up simulations to increase efficiency. I believe writing a journal file is the way forward from what I have read in forums so far. However, I am running transient simulations and I need to save the .dat files every 'x' number of time steps....I also save ppm images at every time step after the 2nd cycle to create an animation.

How can I incorporate these commands ?

Any help would be great !

Many thanks
Vix.
vix is offline   Reply With Quote

Old   November 29, 2012, 00:08
Default Autosave case data files
  #9
New Member
 
Ganapathy Iyer
Join Date: Mar 2009
Location: Pune, Maharashtra, India
Posts: 25
Rep Power: 8
Ganapathy is on a distinguished road
Dear Vix,
You can Autosave dat files, cas files as well as images at various time steps.

/file write autosave allows you to set the values for when you want to auto save the simulation.

You can set up TUI commands in/solve execute commands which will run at fixed timestep / realtime / iterations too
Ganapathy is offline   Reply With Quote

Old   November 29, 2012, 03:57
Default
  #10
Senior Member
 
Marion
Join Date: Jul 2012
Location: France
Posts: 122
Rep Power: 6
Marion is on a distinguished road
Hi Vix,

For autosave you do not need to use the TUI/journals. You can just set it up in Calculation activities/autosave from the GUI.
To save pictures you can use the "execute commands" in the same panel (calculation activities)
Marion.
Marion is offline   Reply With Quote

Old   May 15, 2014, 16:44
Default
  #11
Azy
New Member
 
Azadeh Saeedi
Join Date: Mar 2014
Location: Canada
Posts: 23
Rep Power: 3
Azy is on a distinguished road
Could I ask you a question? for auto saving, the only thing that I need is to create a complete case with auto save, and then run it with the read,iterate commands?
Azy is offline   Reply With Quote

Old   May 15, 2014, 20:16
Default
  #12
kad
Senior Member
 
Join Date: Feb 2013
Location: Germany
Posts: 171
Rep Power: 13
kad will become famous soon enoughkad will become famous soon enough
Quote:
Originally Posted by Azy View Post
Could I ask you a question? for auto saving, the only thing that I need is to create a complete case with auto save, and then run it with the read,iterate commands?
Yes, if you have a entry for autosave in your case file, it is respected while running in batch mode.
Azy likes this.
kad is offline   Reply With Quote

Old   June 2, 2014, 11:02
Default
  #13
Azy
New Member
 
Azadeh Saeedi
Join Date: Mar 2014
Location: Canada
Posts: 23
Rep Power: 3
Azy is on a distinguished road
Thanks alot
Azy is offline   Reply With Quote

Old   June 3, 2014, 05:11
Post Hi
  #14
New Member
 
Anandanarayanan's Avatar
 
Anandanarayanan R
Join Date: May 2013
Location: Coimbatore(TN), India
Posts: 5
Rep Power: 4
Anandanarayanan is on a distinguished road
Hi,
Is there any command that can be used to get a torque value of the rotor(turbomachinery problem) for each time step while solving. Kindly help me.
Anandanarayanan is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Stopping a Fluent batch job AND saving the data! Possible? Volker Pawlik FLUENT 7 May 22, 2014 22:30
Running Job in Batch mode (EFD) Nick Sessions FloEFD, FloWorks & FloTHERM 0 April 16, 2008 16:44
problem with running UDF in batch mode James FLUENT 0 June 6, 2006 06:49
how to convert .par to .geomturbo in batch mode xiaoruofu NUMECA 0 December 30, 2004 05:22
problem with fluent in batch mode Pat FLUENT 2 February 13, 2003 14:14


All times are GMT -4. The time now is 02:28.