[zhixin]

Hi,

I did some transient work using fluent 2020, and the format of the autosave files was .cas.h5.
When I planed to do some post-processing work using CFDpost, I found that the .cas.h5 files could not be opened. I also tested Tecplot, it could not open the file either.
So I was wondering how can I do the post-process work (Besides save the file as .cas).
Any help will be great.

Thanks.

[vinerm]

Case file only contains mesh and setup. Results are in data files. CFDPost may or may not be able to load HDF, but I'd expect Ansys to have made it possible. Else, write data file as dat.gz or export cdat from Fluent.

[zhixin]

Originally Posted by vinerm

Case file only contains mesh and setup. Results are in data files. CFDPost may or may not be able to load HDF, but I'd expect Ansys to have made it possible. Else, write data file as dat.gz or export cdat from Fluent.

Thanks for your reply. Now I have saved new files as the older format. Just wonder why Cfdpost does not support .dat.h5 format.

[piprus]

It's because EnSight does the job instead of CFDPost.
CFD-Post is coming to its end I believe, EnSight was bought just to fill this gap.

[Diconico]

I've faced the same problem. So, that I know, you have two options, if your simulations don't take too long to finish, do them again and create a report for CFD post, or, you can load them in fluent and save in .cas, manually, wich is painfully boring.

[Alexander00]

Originally Posted by Diconico

I've faced the same problem. So, that I know, you have two options, if your simulations don't take too long to finish, do them again and create a report for CFD post, or, you can load them in fluent and save in .cas, manually, wich is painfully boring.

I'm facing the same problem in Ansys 2021 R1 and i want to view result files in techplot but it is not supporting .h5 cas and dat files.
Is there a way to save the result files in simple cas and data files?
please help.

[basil2]

Go to the File->Preferences in the “general” section, change the “Default Format for I/O” from “CFF” to “Legacy”

And then when you write the .cas and .dat files make sure to select the “.cas and .dat” option, and not the CFF format with .cas.h5 and .dat.h5

[wsfowler]

At Tecplot we've just released our Tecplot 360 2021 R1 Beta which includes support for the Ansys Fluent CFF (.cas.h5/.dat.h5) format. The official release should happen by mid-May 2021.

Visit www.tecplot.com and go to the "My Tecplot" link to download the Beta. This requires a portal account, which is free.

Let me know how the loader works for you!

Thanks,
Scott Fowler
Tecplot 360 Product Manager

[kumar.119]

Originally Posted by basil2

Go to the File->Preferences in the “general” section, change the “Default Format for I/O” from “CFF” to “Legacy”

And then when you write the .cas and .dat files make sure to select the “.cas and .dat” option, and not the CFF format with .cas.h5 and .dat.h5

This is the solution to the problem.
Thank you very much!

[shruts]

Where can I find file--> preferences to change the default format?
Is it in the fluent?

[kumar.119]

Here is a link to do so. The same I created to tackle this issue.


https://www.youtube.com/watch?v=uN09vQgkslI&t=81s

[kumar.119]

Originally Posted by shruts

Where can I find file--> preferences to change the default format?
Is it in the fluent?

Use this link to solve your issue:
https://www.youtube.com/watch?v=uN09vQgkslI&t=81s

[hsingtzu]

I found a way to convert .h5 to .dat, which is accepted by CFD-POST.
I will explain with an example, say there are two files, FFF.gz.cas.h5 and FFF.gz.1.dat.h5.

1. Open “FFF.gz.cas.h5” using Fluent
2. File>Read>Data, choose “FFF.gz.1.dat.h5”
3. File>Write>Case and Data, choose where you like to save the files and click “OK”
4. Repeat 2. and 3. as needed
5. Open CFD-POST
6. Load Results file, choose either “FFF.gz.1.dat” or “FFF.gz.1.cat” to do postprocessing

[zemfahs]

Originally Posted by kumar.119

Here is a link to do so. The same I created to tackle this issue.


https://www.youtube.com/watch?v=uN09vQgkslI&t=81s

Thanks for this information. I watched this video but Ansys Fluent 2020 R2 doesn't have "default format for I/O" (only this option is absent).
When I export the data as Tecplot it gives an error as "Zone ID 18 in file "file.cas" has no nodes." I used Watertight Geometry mesh type in 3D. I couldn't get any images from the Tecplot. I've tried to save it with all kind of formats (including Ensight), however generally it gives an error about the mesh type "polyhexcore".

Has anyone encountered this error?

[wsfowler]

zemfahs,

Are you able to use Tecplot 360's Fluent CFF (*.h5) data loader to load cas.h5/dat.h5 files directly? This data loader was introduced in Tecplot 360 2021 R1 (May 2021)

Thanks,
Scott

[zemfahs]

Thanks for answering wsfowler,
My fluent (2020 R2) doesn't save as .cas.h5 or dat.h5. It saves as .cas and .dat.
I also tried Tecplot 2022 version but it didn't work.

I have a 3D model in ANSYS 2020 R2. I ran it and got my results which were correct. But when I save my analysis as TEC file and try to open it with Tecplot 360 it looks like 2D. Then when I select 3D Cartesian it opens but this time Iso-Surfaces is passive. As far as I understand, the program assumes that my file is 2D. Because the program only sees the models sides, top, bottom, inlet and outlet. it can not see interior.

Then as a second way, I saved the data as .cas and .dat to open the file in Tecplot. However this time in Tecplot there is another error message for me 'Zone ID 44 in file "file.cas" has no nodes.'

[wsfowler]

My understanding is that Ansys Fluent only exports the surface data when writing to Tecplot format. Tecplot 360 will load this data in 2D mode since there are no volume elements in the dataset. You can flip to a 3D view using the Plot Type control at the top-left of the user interface.

I'm concerned though that Tecplot 360 is having problems loading your .cas and .dat files. We should be able to load these files. If you're able to share your data with our support staff, that would be ideal - perhaps there's an issue with our data loader. Please contact support@tecplot.com.

Thanks,
Scott

[Abbas Dorri]

very nice. My problem was also solved.

[saideh]

I have a problem with loading the saved sequences all to the cfd post to have the evolution in time... it doesn't load it as all saved data files and keeps them all seperated. also, i chose the option to keep it as single case