Fluent Batch Mode - TUI
 

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

Hi,
Can you post a copy of the script you are using here? It would be easier to see if there are errors.
Marion.

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

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.

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.

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

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

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.

Autosave case data files
 

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

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.

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.

Thanks alot :)

Hi
 

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.