[saisanthoshm88]

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

[Far]

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

[brunoc]

Originally Posted by saisanthoshm88

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.

[Far]

Originally Posted by brunoc

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

[brunoc]

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.

[ghorrocks]

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

[Crank-Shaft]

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.

[villager]

Originally Posted by brunoc

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.

[sihaqqi]

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

[puneetnema]

Originally Posted by Far

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..?

[ghorrocks]

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.

[puneetnema]

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

[chandrasekhar]

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

Originally Posted by ghorrocks

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]

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

[villager]

Originally Posted by ghorrocks

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.

Originally Posted by chandrasekhar

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

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.

[Zerzura]

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

[hfalleiro]

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

[brunoc]

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.

[hfalleiro]

Thanks for the information

[csystudio]

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

Enjoy!