CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Can I load FLUENT time mean data into CFD-Post? (

ivanbuz September 21, 2010 21:08

Can I load FLUENT time mean data into CFD-Post?
Hi All,

When I load Fluent case and data files into CFD-POST, I can only see the results of the final time step. But I also have time-averaged results in my FLUENT data file, how can I see them in CFD-post?

Thanks a bunch!


ivanbuz September 23, 2010 08:20

Anybody can give me some help?

I wrote time-mean results ( Unsteady Statistics) in the Fluent data file. My question is how to load those time-mean data into CFD-Post. All I can see in CFD-Post are data for only a time instance, not time-mean.

Thank you guys!


physix July 26, 2012 07:21

I know this thread is old, but I believe many people are stuck with the same problem.
My workaround:
Open the .cas and .dat file in FLUENT and then go to file > export to CFD-Post and select the mean variables there. CFD-Post is then able to read the variables from the .cdat file.

vmlxb6 September 25, 2012 10:30

@ ivanbuz
The question actually is how to load all the different .cas and .dat files into cfd post for animation.
I had used CFX previously and loaded all the .trn files together for animation but I am now using Fluent and would like to know how to load all the .dat files together for animation.

When I use the ctrl button to select multiple files, they all open up in different windows ?

villager February 21, 2013 16:30

Ok, they really open in new windows, if you say them to do so :)
Seriously, you should follow these instructions:
1) Go to "Calculate Activities" in the left menu (Problem Setup) of FLUENT in your transient FLUENT calculation case file (before calculation!).
2) Under "Automatic Export" choose Create -> Solution Data Export.
3) Choose file type "CFD-Post compatible", format - binary or ASCII (as u like)
4) At right you'll see panel Quantities - here you should select with mouse-probe button variables, that you like to postprocess in CFD-Post. These variables will be written to file at every n-th time-step, value of "n" is selected under Frequency (Time Steps) in this dialog box.
NOTE: Your casefile filename MUSTN'T contain dots ('.') Otherwise, you'll have big problems with renaming files after calculations to watch all timesteps at one place.
5) Do your unsteady calculations
6) Open CFD-Post manually or from FLUENT (File -> Export to CFD-Post.. here you must specify filename (arbitrary) )
7) In CFD-Post: File -> Load Results
8) Here you should specify your first timestep case.
Bruno noted that casefiles from other timesteps (if any) should be moved to another directory.
9) Choose "Load complete history as -> A single case" at right.
10) After loading, Tools -> TimeStep Selector -> you should see all timesteps (a number of partial and the final).
The common problems are: ignoring NOTE from "4)", ignoring "9)".
P.S. :) This could be helpful:
FLUENT 12.1 - Unsteady Flow Past a Cylinder - Results
Good luck.

razi.me05 September 11, 2014 05:46

Hi, i did a transient problem but i didn't save a case file. I have the data set only. Can I do simulation without a case file or will I have to run all the simulations again. Please help. I've done a lot of simulations. Doing those again is really almost impossible.

why? April 16, 2015 01:51

With this method the particle data is not exported. You can only select the continuous phase data when exporting a cdat file from fluent. The particle data is supposed to be exported separately.

I have been trying to export it and fluent writes a xml file which is readable to CFDPost but gives the particle data at one position.

Anyone here knows how to import the particle trajectories from Fluent into CFD post. Fluent can do this when running in GUI where you can save an animation file but I am running my simulations on a cluster and all I get is a 2 kb xml file which doesnt really have any particle data in it.

spggodd April 7, 2016 16:34

I have imported as villager suggests but every time step appears to be almost the same when I was expecting some sort of vortex shedding.

The time steps all say "Partial" is this an issue?

Any ideas?

All times are GMT -4. The time now is 19:41.