Animation of Fluent transient data
 

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

Use Techplot or Fieldview for this purpose. But I also believe there should be option in CFD-Post but I never used it.

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

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.

CFX has this capability as well (reduced size output files for transient runs) - you can select what variables go into a trn file.

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.

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.

sir how can i do it in techplot..?

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.

Sir i tried in CFD-Post also,bur not able to do it..can u plz help regarding the way it should be done.

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

It sounds like you are using Fluent - try the Fluent forum.

Yes, but the topic is : "Animation of Fluent transient data". I suppose moving the thread to the FLUENT forum.

Here is a nice example
http://www.cfd-online.com/Forums/flu...tml#post348225
adding %t to the filename solves the problem.

Also, you can use %i (iteration number) %n (sequential file number) from helpful A. Bakker's notes.

animation CFD-post does not work
 

Dear all,

I saved my files with filename-0.100.dat, filename-0.200.dat etc. But still in CFD-post the time is not recognized. All my files get the same time.
I load the files as 'single history' with one .cas file and multiple .dat files.

Please if you can help me I would be very happy :).

Kind regards,
Madelon

Hi Bruno,
Can you tell me how to save the files in .cdat.

On Calculation Activities, create an Automatic Export using File Type = CFD-Post Compatible.

Set the export frequency, file name, etc. If your mesh doesn't change, disable Write Case File Every Time. But do save case/data files whenever you quit or restart the solver.

Thanks for the information

This is the way to do it in CFD-Post:
http://www.eureka.im/downloads/faq215_KR215.pdf

Enjoy!

Dear sir,

Thank you so much! I'm running a LOT of transient data for my thesis, and loading that one-a-one was just impossible... Now I can do a proper animation and get transient data! As you can imagine, I didn't setup the autosave before starting, and now it's too late to run everything again... Any way in CFD-Post to time-average the multiple solutions? I've got all the .dat and .cas files, for each time step.

Once again, thank you SO much!

CFD-Post cannot do time averaging to my knowledge. Have a look around but I don't think it can.

Don't forget you can automate repetitive actions in CFD-Post with session files.

Yeah, but my post is simple: just a few points measuring velocity u and plots of Q criterion vortex Core surface... Maybe I'll do the averaging on Matlab or Fortran, seems easier anyways... Do you know the TUI command to setup data sampling? I'm used to running fluent using it's GUI, only recently I needed to create a journal for cluster run...

Thank you!

Sent from my XT1635-02 using CFD Online Forum mobile app