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

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

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

Like Tree6Likes
  • 1 Post By ivanbuz
  • 1 Post By physix
  • 4 Post By villager

LinkBack Thread Tools Search this Thread Display Modes
Old   September 21, 2010, 21:08
Default Can I load FLUENT time mean data into CFD-Post?
Join Date: May 2009
Posts: 85
Rep Power: 17
ivanbuz is on a distinguished road
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 is offline   Reply With Quote

Old   September 23, 2010, 08:20
Join Date: May 2009
Posts: 85
Rep Power: 17
ivanbuz is on a distinguished road
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!

roi247 likes this.
ivanbuz is offline   Reply With Quote

Old   July 26, 2012, 07:21
Default Workaround
New Member
Join Date: Jul 2012
Posts: 1
Rep Power: 0
physix is on a distinguished road
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.
masoud.ravan likes this.
physix is offline   Reply With Quote

Old   September 25, 2012, 10:30
Default @ ivanbuz
Senior Member
Ugly Kid Joe
Join Date: Aug 2010
Posts: 193
Rep Power: 15
vmlxb6 is on a distinguished road
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 ?
vmlxb6 is offline   Reply With Quote

Old   February 21, 2013, 15:30
Smile Answer
Join Date: Jul 2011
Location: My home :)
Posts: 81
Rep Power: 18
villager is on a distinguished road
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.
villager is offline   Reply With Quote

Old   September 11, 2014, 05:46
Join Date: Apr 2014
Posts: 32
Rep Power: 12
razi.me05 is on a distinguished road
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.
razi.me05 is offline   Reply With Quote

Old   April 16, 2015, 01:51
New Member
Join Date: Apr 2015
Posts: 16
Rep Power: 11
why? is on a distinguished road
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.
why? is offline   Reply With Quote

Old   April 7, 2016, 16:34
Steven Goddard
Join Date: Mar 2015
Posts: 34
Rep Power: 11
spggodd is on a distinguished road
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?
spggodd is offline   Reply With Quote


cfd-post, fluent

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
AMI speed performance danny123 OpenFOAM 21 October 24, 2020 04:13
Extrusion with OpenFoam problem No. Iterations 0 Lord Kelvin OpenFOAM Running, Solving & CFD 8 March 28, 2016 11:08
simpleFoam error - "Floating point exception" mbcx4jc2 OpenFOAM Running, Solving & CFD 12 August 4, 2015 02:20
Star cd es-ice solver error ernarasimman STAR-CD 2 September 12, 2014 00:01
mixerVesselAMI2D's mass is not balancing sharonyue OpenFOAM Running, Solving & CFD 6 June 10, 2013 09:34

All times are GMT -4. The time now is 16:07.