CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Post-Processing (http://www.cfd-online.com/Forums/openfoam-post-processing/)
-   -   FoamDataToFluent (http://www.cfd-online.com/Forums/openfoam-post-processing/61340-foamdatatofluent.html)

maritozzo October 6, 2005 05:41

Someone can tell me what i nee
 
Someone can tell me what i need to specify in the foamDataTofluent controlDict..
Please Help

hjasak October 6, 2005 06:27

There is an example dictionary
 
There is an example dictionary shipped with the application and this should be the case for ALL such dictionaries. Have a look at:

OpenFOAM-1.2/applications/utilities/postProcessing/dataConversion/foamDataToFlue nt

There, you will find the example dictionary: foamDataToFluentDict, a list of fluent unit numbers that are given in the converter and the complete source code.

Hrv

nfoxley May 10, 2006 10:40

Hi, I have used the templat
 
Hi,

I have used the template suggested above but I still only get the mesh for t=0. I am using OF v1.2, will v1.3 be any different?

Thanks, Natalie

hjasak May 10, 2006 11:13

It still works in OpenFOAM-1.3
 
It still works in OpenFOAM-1.3 as it did in 1.2 - I have just tested it:

1) edit system/controlDict and set

startFrom latestTime;

2) run:

foamMeshToFluent /home/hjasak/OpenFOAM/hjasak-1.3/run/test cavity

3) run:

foamDataToFluent /home/hjasak/OpenFOAM/hjasak-1.3/run/test cavity

4) look at the data:

cd /home/hjasak/OpenFOAM/hjasak-1.3/run/test/cavity/fluentInterface
fluent 3d

and load the case and data.

Hrv

nfoxley May 10, 2006 12:19

Hi again, I have done what
 
Hi again,

I have done what you suggested above. I can now get the log file to say that it is writing at the the latest time, but the resulting data is nonsense as it is just zeros, which is not in agreement with the output for paraFoam, EnSight or VTK for the same case. I have tried on 3 different cases and the result is always the same. Also, is there no way to write data at every timestap as there is for the other post processors?

Thanks,
Natalie.

hjasak May 10, 2006 13:12

Hi Natalie, (copy of E-mail)
 
Hi Natalie, (copy of E-mail)

I have packed and attached the case - could you please try this one to see if your installation works.

As for multiple steps, you can easily change the code: just take the contents of the foamDataToFluent and put it all into a time loop. Additionally, dump every set of results into a separate file and all should be well on the Fluent side.

If you need help with this, please give me a shout and I'll help.

Regards,

Hrv

nfoxley May 11, 2006 13:03

Hi, Thank you for the abov
 
Hi,

Thank you for the above... that reads into fluent fine and I can reproduce the results...2nd time around. I seem to have a problem where running foamDataToFluent sometimes overwrites my data with something similar to (but not the same as) the conditions at t=0. I have not been able to isolate under which circumstances it does this and when it doesn't. I have found that using the backup files I can resave my data and try again, then it usually works. Why is this the case?

I'll try your suggestion for attempting multiple steps in the next few days,

Thanks again,
Natalie.

vivekcfd February 22, 2007 08:03

Hi I am facing exactly the sa
 
Hi
I am facing exactly the same problem. I am trying to convert the cavity case with foamDataTofluent, however, the output file contains field value 0 everywhere. Hrv could you pls let me know, how to overcome this problem? I want to convert Foam data to Fluent.

thanks
Vivek

hjasak February 22, 2007 09:57

Have a look at your controlDic
 
Have a look at your controlDict: does it by any chance say:

startFrom startTime;
startTime 0;


If you've got zeros, it is likely that you are converting startTime instead of latestTime or similar, which actually contains the results.

Give me a sign,

Hrv

vivekcfd February 23, 2007 03:09

my controlDict says: startF
 
my controlDict says:

startFrom firstTime;
startTime 0;

I think you are right, the problem is that I am getting file corresponding to startTime, i.e. 0.

Could you please let me know how to solve the problem?

thanks

hjasak February 23, 2007 03:28

Do you have any results? What
 
Do you have any results? What is the time directory you wish to use? Put that number under startTime.

Alternatively, do startFrom latestTime; which should do the trick.

Hrv

robinp September 5, 2007 11:16

I'm also getting the problem w
 
I'm also getting the problem with foamDataToFluent writing a load of zeros instead of the data I've created. I've checked the data previously with paraFOAM, so I know it's there, but the act of running foamDataToFluent overwrites the data with zeros before converting it to the Fluent mesh. I've played around with the start time, and as a result have managed to erase my data at several time steps. Has anyone managed to sort out this problem yet?

robinP

hjasak September 5, 2007 11:23

Heya, At the beginning of f
 
Heya,

At the beginning of foamDataToFluent.C it says:

Info<< "Time = " << runTime.timeName() << nl << endl;

Therefore, the code should tell you which time-step it is using to read. Could you check that the numbers in the fields for that time are correct and that this is what you are actually trying to convert.

The second issue is the contents of foamDataToFluentDict: this gives you the Fluent field code for each named field you are trying to convert. Do you have that/does it make sense? You could also manually check the resulting .cas file to see if there are numbers in there to establish if it is the converter causeing trouble or the subsequent read into Fluent.

Hrv

robinp September 6, 2007 12:40

The program was accessing the
 
The program was accessing the correct timestep, where there was data before I ran it, but it was overwritten with zeros by the time it finished. That said, I reran my case to replace the data and it did work today, despite me making no discernable changes. This seems to be the same problem reported by Natalie Foxley on May 11, 2006, above. I'm using Xfoam to run foamDataToFluent so the foamDataToFluentDict is the one set up on the fly by the GUI. I'm just using the defaults, but they're the same as in the user guide.

Robin

lhcamilo December 23, 2008 06:41

I have followed the instructio
 
I have followed the instructions above to export foam files into fluent format, though mostly it works (I am able to get the .dat files for each time step), I can't seem to find the .cas file(s) inside the "fluentInterface" folder.


any tips?

thanks in advance

leo

fra76 December 23, 2008 08:38

foamDataToFluent, as the name
 
foamDataToFluent, as the name says, exports only the data files.
You need to run foamMeshToFluent as well.

Francesco

lhcamilo December 23, 2008 09:25

thank for the reply, though fo
 
thank for the reply, though foamMeshToFluent did produce a .msh file, it seems I still need a .cas file to read it into Tecplot.

I have already tried, to import foam cases first into tecplot using the foamToTechplot tool but that cannot handle the polyhedrals that are generated by snappy , then the Ensight one (breaks Tecplot 360 2008, I have already contacted the support and I am waiting their response.).

any further help is greatly appreciated

regards

leo

fra76 December 23, 2008 13:02

If you have access to fluent,
 
If you have access to fluent, just load the .msh and save it as .cas.
Otherwise you could try to rename the .msh in .cas and cross your fingers! The main difference between the two is the boundary conditions sections, only present in the .cas file. The mesh is the same in both files.
I don't know Tecplot at all, so this is all I can suggest you.

Francesco

khalid1059 September 28, 2009 01:15

Quote:

Originally Posted by maritozzo (Post 199327)
Someone can tell me what i need to specify in the foamDataTofluent controlDict..
Please Help

Hi a m a new OpenFOAM user. can u plzz tell me in detail How OpenFOAM data is conveted to Fluent as a single Fluent.dat file. I tried the command foamDataToFluent but as a result i got plenty of files for fluent for each time step for transient case. Now i dont know how to read them in fluent.:eek:Bcz in fluent only a single .dat file is to be needed for reading but here are plenty of .dat files.I m in a fix plzz resolve my problem:(:(

gschaider September 28, 2009 12:30

Quote:

Originally Posted by khalid1059 (Post 230662)
Hi a m a new OpenFOAM user. can u plzz tell me in detail How OpenFOAM data is conveted to Fluent as a single Fluent.dat file. I tried the command foamDataToFluent but as a result i got plenty of files for fluent for each time step for transient case. Now i dont know how to read them in fluent.:eek:Bcz in fluent only a single .dat file is to be needed for reading but here are plenty of .dat files.I m in a fix plzz resolve my problem:(:(

The last time I worked with Fluent (admittedly some time ago) it wrote a .dat-file for every time-step (maybe this changed with the newest versions). So this sounds more like a Fluent problem and I guess the Fluent-support will be happy to help you with this


All times are GMT -4. The time now is 01:13.