CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

How to use DESModelRegions function object

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

Like Tree4Likes
  • 4 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   May 1, 2013, 18:37
Default How to use DESModelRegions function object
  #1
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 5
hakonbar is on a distinguished road
Hi! I'm doing some DES simulations, and I would like to see which parts of my flow field are in RANS mode and which are in LES mode. I see the new OF release (2.2.0) introduced a new function object called DESModelRegions, which outputs this data. The thing is, I don't know which lines to put in the controlDict in order to activate this object, and which library to load.

Have any of you used this function object before, and do you know which libs to load etc?

best regards,
Håkon Line
hakonbar is offline   Reply With Quote

Old   May 2, 2013, 08:48
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,531
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Håkon,

Without an example case, I can't test any further than the following instructions:
  1. Edit the file "system/controlDict".
  2. Append/add the following block:
    Code:
    functions
    {
        desField
        {
            type            DESModelRegions;
            functionObjectLibs ("libutilityFunctionObjects.so");
            log             true;
            //region "region0";
            enabled on;
            storeFilter on;
            timeStart 0.0;
            timeEnd 10.0;
            outputControl timeStep;
            outputInterval       5000;
        }
    }
    Note: it writes and outputs information for each 5000 steps in this example! And if you do not define the "timeStart" and "timeEnd", it will run for the whole simulation.
  3. It created the file "postProcessing/desField/0/DESModelRegions.dat", but I didn't use DES, so I only got this header:
    Code:
    # DES model region coverage (% volume)
    # time  LES     RAS
  4. And since I used "log true;", I only got this message:
    Code:
    DESModelRegions output:
        No DES turbulence model found in database
  5. And it creates the field "DES::LESRegion".
Like I wrote at the beginning, without an example, I can't test this properly.

edit: I do have an example case now and is used here: Problems with IDDES in openfoam2.1.1 - post #10

Best regards,
Bruno
__________________

Last edited by wyldckat; May 2, 2013 at 15:13. Reason: I've updated the post with new information and see "edit:"
wyldckat is offline   Reply With Quote

Old   May 3, 2013, 08:15
Default
  #3
New Member
 
Håkon Bartnes Line
Join Date: Mar 2013
Posts: 27
Rep Power: 5
hakonbar is on a distinguished road
It works perfectly, thanks! Now I've learned the general syntax for function objects as well. =)
hakonbar is offline   Reply With Quote

Old   July 5, 2016, 07:26
Default
  #4
New Member
 
Peter
Join Date: Nov 2015
Location: Hamburg, Germany
Posts: 27
Rep Power: 2
potentialFoam is on a distinguished road
Dear Foamers,

can you help me to use 'DESModelRegions' with OF30X?

I fear, it is not implemented in OF30X. But how could you determine the RANS content of a DES?

Using an older version (like OF231) for postprocessing does not work, 'cos the constant/turbulenceProperties-file changed since this version.

Even this thread
HTML Code:
http://www.cfd-online.com/Forums/openfoam-solving/104123-les-content-detached-eddy-simulation-openfoam.html
does not provide an answer for OF30X.

I would be happy to hear your ideas!
Regards,
Peter

EDIT:
According to a hint I installed OpenFOAM-v1606+ from openfoam.com
and this perfectly works for postprocessing cases simulated with OF301 :-)

Last edited by potentialFoam; July 6, 2016 at 03:47.
potentialFoam 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
foamToTecplot360 thomasduerr OpenFOAM Post-Processing 111 April 5, 2016 21:28
OpenFOAM static build on Cray XT5 asaijo OpenFOAM Installation 9 April 6, 2011 12:21
ParaView for OF-1.6-ext Chrisi1984 OpenFOAM Installation 0 December 31, 2010 07:42
Is function object forceCeofficient compatible with interDyMFoam? Philer OpenFOAM Running, Solving & CFD 0 March 10, 2010 11:30
Error with Wmake skabilan OpenFOAM Installation 3 July 28, 2009 00:35


All times are GMT -4. The time now is 01:17.