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

FoamDataToFluent

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

Like Tree8Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 6, 2005, 05:41
Default Someone can tell me what i nee
  #1
Member
 
Muzio Grilli
Join Date: Mar 2009
Posts: 36
Rep Power: 9
maritozzo is on a distinguished road
Someone can tell me what i need to specify in the foamDataTofluent controlDict..
Please Help
maritozzo is offline   Reply With Quote

Old   October 6, 2005, 06:27
Default There is an example dictionary
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,781
Rep Power: 22
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 10, 2006, 10:40
Default Hi, I have used the templat
  #3
nfoxley
Guest
 
Posts: n/a
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
  Reply With Quote

Old   May 10, 2006, 11:13
Default It still works in OpenFOAM-1.3
  #4
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,781
Rep Power: 22
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 10, 2006, 12:19
Default Hi again, I have done what
  #5
nfoxley
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   May 10, 2006, 13:12
Default Hi Natalie, (copy of E-mail)
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,781
Rep Power: 22
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 11, 2006, 13:03
Default Hi, Thank you for the abov
  #7
nfoxley
Guest
 
Posts: n/a
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.
  Reply With Quote

Old   February 22, 2007, 08:03
Default Hi I am facing exactly the sa
  #8
Member
 
Vivek Kumar
Join Date: Mar 2009
Location: Switzerland
Posts: 34
Blog Entries: 1
Rep Power: 9
vivekcfd is on a distinguished road
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
vivekcfd is offline   Reply With Quote

Old   February 22, 2007, 09:57
Default Have a look at your controlDic
  #9
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,781
Rep Power: 22
hjasak will become famous soon enough
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
mm.abdollahzadeh likes this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   February 23, 2007, 03:09
Default my controlDict says: startF
  #10
Member
 
Vivek Kumar
Join Date: Mar 2009
Location: Switzerland
Posts: 34
Blog Entries: 1
Rep Power: 9
vivekcfd is on a distinguished road
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
vivekcfd is offline   Reply With Quote

Old   February 23, 2007, 03:28
Default Do you have any results? What
  #11
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,781
Rep Power: 22
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 5, 2007, 11:16
Default I'm also getting the problem w
  #12
New Member
 
Robin Pitt
Join Date: Mar 2009
Posts: 4
Rep Power: 9
robinp is on a distinguished road
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
robinp is offline   Reply With Quote

Old   September 5, 2007, 11:23
Default Heya, At the beginning of f
  #13
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,781
Rep Power: 22
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 6, 2007, 12:40
Default The program was accessing the
  #14
New Member
 
Robin Pitt
Join Date: Mar 2009
Posts: 4
Rep Power: 9
robinp is on a distinguished road
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
robinp is offline   Reply With Quote

Old   December 23, 2008, 06:41
Default I have followed the instructio
  #15
Member
 
Leonardo Honfi Camilo
Join Date: Mar 2009
Location: Delft, Zuid Holland, The Netherlands
Posts: 48
Rep Power: 9
lhcamilo is on a distinguished road
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
lhcamilo is offline   Reply With Quote

Old   December 23, 2008, 08:38
Default foamDataToFluent, as the name
  #16
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 219
Rep Power: 10
fra76 is on a distinguished road
foamDataToFluent, as the name says, exports only the data files.
You need to run foamMeshToFluent as well.

Francesco
fra76 is offline   Reply With Quote

Old   December 23, 2008, 09:25
Default thank for the reply, though fo
  #17
Member
 
Leonardo Honfi Camilo
Join Date: Mar 2009
Location: Delft, Zuid Holland, The Netherlands
Posts: 48
Rep Power: 9
lhcamilo is on a distinguished road
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
lhcamilo is offline   Reply With Quote

Old   December 23, 2008, 13:02
Default If you have access to fluent,
  #18
Senior Member
 
Francesco Del Citto
Join Date: Mar 2009
Location: Zürich Area, Switzerland
Posts: 219
Rep Power: 10
fra76 is on a distinguished road
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
fra76 is offline   Reply With Quote

Old   September 28, 2009, 01:15
Default
  #19
New Member
 
Syed khalid Hussain Shah Hashmi
Join Date: Jul 2009
Location: Lahore, Pakistan
Posts: 5
Rep Power: 9
khalid1059 is on a distinguished road
Quote:
Originally Posted by maritozzo View Post
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.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
khalid1059 is offline   Reply With Quote

Old   September 28, 2009, 12:30
Default
  #20
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,920
Rep Power: 41
gschaider will become famous soon enoughgschaider will become famous soon enough
Quote:
Originally Posted by khalid1059 View Post
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.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
gschaider 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
FoamDataToFluent dnomdec OpenFOAM Post-Processing 8 July 31, 2013 11:07
Error whit foamDataToFluent matteo_gautero OpenFOAM 1 November 12, 2012 05:46
Velocity Components in foamDataToFluent flavio_pergolesi OpenFOAM Post-Processing 1 November 9, 2009 10:27
FoamDatatoFluent BC achuneka OpenFOAM Post-Processing 4 August 16, 2008 11:21
FoamDataToFluent Problem aganesan OpenFOAM Post-Processing 8 June 4, 2008 17:15


All times are GMT -4. The time now is 01:50.