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

Animation of Fluent transient data

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

Like Tree4Likes
  • 2 Post By brunoc
  • 2 Post By Crank-Shaft

Reply
 
LinkBack Thread Tools Display Modes
Old   December 16, 2012, 05:46
Default Animation of Fluent transient data
  #1
Senior Member
 
---------
Join Date: Oct 2010
Posts: 296
Rep Power: 8
saisanthoshm88 is on a distinguished road
I need to create an animation out of a transient solution data from Fluent.

There are many transient files to be considered to produce the animation.

If I create a solution animation in the calculation activities I wonder if the simulation would take long as the animation commands need to be executed at many time steps when the simulation is proceeding. ( I just started up with Fluent so this is how I know to do it)

Isn't there a way to produce such animation after the simulation is finished.

Taking a snapshot of each transient file data is not possible as there are many.

I tried to use CFD Post but fluent transient data is not supported in it's time step selector.

Could some one please suggest a better way of doing this
__________________
Best regards,
Santhosh.

Last edited by saisanthoshm88; December 16, 2012 at 14:15.
saisanthoshm88 is offline   Reply With Quote

Old   December 16, 2012, 05:54
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Use Techplot or Fieldview for this purpose. But I also believe there should be option in CFD-Post but I never used it.
Far is offline   Reply With Quote

Old   December 17, 2012, 11:01
Default
  #3
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 224
Rep Power: 10
brunoc is on a distinguished road
Quote:
Originally Posted by saisanthoshm88 View Post
I tried to use CFD Post but fluent transient data is not supported in it's time step selector.

Could some one please suggest a better way of doing this
Actually CFD Post does support FLUENT transient files, but you should open a dat file that uses the FLUENT transient naming conventions, that is, filename-XXXXX.dat, where XXXXX is the timestep number. Your cas file should be named filename.cas (without the timestep number). If you have other cas files with the timestep number, try moving them to another folder.

I use it here a lot and it works fine.

Cheers.
villager and meh22 like this.
brunoc is offline   Reply With Quote

Old   December 17, 2012, 11:11
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by brunoc View Post
Actually CFD Post does support FLUENT transient files, but you should open a dat file that uses the FLUENT transient naming conventions, that is, filename-XXXXX.dat, where XXXXX is the timestep number. Your cas file should be named filename.cas (without the timestep number). If you have other cas files with the timestep number, try moving them to another folder.

I use it here a lot and it works fine.

Cheers.
Good info . Thanks for sharing
Far is offline   Reply With Quote

Old   December 17, 2012, 12:11
Default
  #5
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 224
Rep Power: 10
brunoc is on a distinguished road
For future simulations, I should add that FLUENT has an option to export what it call cdat files, which are dat files with a reduced number of fields and that can be read in CFD Post. They work like a CFX trn file and their main advantage is saving up space when running a large transient simulation.
brunoc is offline   Reply With Quote

Old   December 17, 2012, 16:23
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,551
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX has this capability as well (reduced size output files for transient runs) - you can select what variables go into a trn file.
ghorrocks is offline   Reply With Quote

Old   December 18, 2012, 18:34
Default
  #7
Senior Member
 
Crank-Shaft's Avatar
 
Ovi
Join Date: Oct 2012
Location: Sydney, Australia
Posts: 121
Rep Power: 4
Crank-Shaft is on a distinguished road
When using Fluent solver for the simulation, I generally select the option to automatically save a file every x number of time-steps. This saves a cdat file for every the time-steps and when the results case file is opened in CFD Post you are able to select the option to 'open entire history as a single case'.

I don't always use this feature but it is really helpful when you are trying to visualise the evolution of the flow field. When the complete history is loaded into CFD Post you are able to select your instance through the 'time-step selector' and this further leads into keyframe animations.

If the storage capacity is a concern you can always choose to save the results for every 2, 5 or 10 time-steps and this will reduce the total amount of data collected.
rgd and yashganatra like this.
__________________
--
Mechanical Engineering
Sydney, Australia


Crank-Shaft is offline   Reply With Quote

Old   February 21, 2013, 15:39
Smile
  #8
Member
 
John M.
Join Date: Jul 2011
Posts: 52
Rep Power: 5
villager is on a distinguished road
Quote:
Originally Posted by brunoc View Post
Actually CFD Post does support FLUENT transient files, but you should open a dat file that uses the FLUENT transient naming conventions, that is, filename-XXXXX.dat, where XXXXX is the timestep number. Your cas file should be named filename.cas (without the timestep number). If you have other cas files with the timestep number, try moving them to another folder.

I use it here a lot and it works fine.

Cheers.
Your casefile filename MUSTN'T contain dots ('.') Otherwise, you'll have problems with renaming files, because FLUENT will create smth like that:
filename-foo-XXXXX.barbaz.cdat
and CFD-Post won't be able to understand filenames as timesteps, because of your filename symbols after your dot.
In linux, for renaming files, use this command:
rename 's/\.barbaz*//' *.barbaz*
It's recommended to enter this command before renaming:
ls *.barbaz*
to be sure, you are renaming only timestep files. Otherwise, move unwanted files to another dir.
villager is offline   Reply With Quote

Old   November 15, 2013, 20:12
Default
  #9
Senior Member
 
starter
Join Date: Sep 2012
Posts: 106
Rep Power: 6
sihaqqi is on a distinguished road
Dear Sir
Since transient data from Fluent is being discussed, can you kindly advise on the following issue.
I am having this strange error in Ansys during FSI. I am using Fluent and Transient Structural. Main source of error occurs in Analysis settings while defining time steps. When I run in Fluent for initial time step of 0.0001 and final step of 0.1s, and import loads in transient using WB, the Analysis settings in transient structural wants to have final time of value of 1. Though this shall never be the case but for the purpose of testing, when I run Fluent for time steps finishing at 5 seconds, it again gives the message that inaccurate time step has been selected. It only solves with extremely large displacements for time value of 1 and due to this lot of non-convergence is happening as it starts giving me erroneous results. I have visited this link http://www.eureka.im/4470.html which tells the method to address this situation but when I open this file, all values that I get are 1 at the place in the file mentioned. I have almost tried for the last two weeks to resolve this but to no avail. My final settings for extremely fine mesh shall be 0.15 at very best. If I have to increase the time step to 1 in Fluent, my calculation time will increase drastically as both geometries I have to evaluate are very big.

Regards


sihaqqi is offline   Reply With Quote

Old   December 1, 2013, 08:47
Default
  #10
New Member
 
Puneet
Join Date: Sep 2013
Posts: 13
Rep Power: 3
puneetnema is on a distinguished road
Quote:
Originally Posted by Far View Post
Use Techplot or Fieldview for this purpose. But I also believe there should be option in CFD-Post but I never used it.
sir how can i do it in techplot..?
puneetnema is offline   Reply With Quote

Old   December 1, 2013, 16:27
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,551
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This is the CFX forum - try a tecplot forum for questions on tecplot.

But note that brunoc's post #3 where he says it can be easily done in CFD-Post as well. There is no need to go to tecplot for post processing.
ghorrocks is offline   Reply With Quote

Old   December 2, 2013, 02:45
Default
  #12
New Member
 
Puneet
Join Date: Sep 2013
Posts: 13
Rep Power: 3
puneetnema is on a distinguished road
Sir i tried in CFD-Post also,bur not able to do it..can u plz help regarding the way it should be done.
puneetnema is offline   Reply With Quote

Old   March 20, 2014, 22:07
Default
  #13
New Member
 
Chandrasekhar
Join Date: Oct 2013
Location: new jersey
Posts: 21
Rep Power: 2
chandrasekhar is on a distinguished road
Hi
i have to store xy plots for each time step, i tried using executive commands but the since the file name does not change in a executive command it gets overwritten. i would like to know if a scheme file can written to do this job. also if its possible i would like to know how to write it (i am not familiar with scheme). Any help on this would be appreciated. Many thanks for replying.

with regards


Quote:
Originally Posted by ghorrocks View Post
This is the CFX forum - try a tecplot forum for questions on tecplot.

But note that brunoc's post #3 where he says it can be easily done in CFD-Post as well. There is no need to go to tecplot for post processing.
chandrasekhar is offline   Reply With Quote

Old   March 21, 2014, 05:24
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,551
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It sounds like you are using Fluent - try the Fluent forum.
ghorrocks 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
Problem converting fluent mesh vinz OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 20 November 17, 2012 10:54
FLUENT can not read data file jing113cn FLUENT 0 December 6, 2010 09:06
animation in fluent doki FLUENT 0 June 10, 2010 08:04
How to update polyPatchbs localPoints liu OpenFOAM Running, Solving & CFD 6 December 30, 2005 17:27


All times are GMT -4. The time now is 18:03.