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

fvOptions: temperatureLimitsConstraint or limitTemperature not working on V3.0+

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 31, 2016, 12:35
Default fvOptions: temperatureLimitsConstraint or limitTemperature not working on V3.0+
  #1
Senior Member
 
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 13
derekm is on a distinguished road
moving from 2.4.0 to 3.0+ and the fvOption temperatureLimitsConstraint has been removed.is this a bug or policy? I've checked the src and it is definitely gone.

edit/
I 've subsequently found out its deliberate in 3.0. however in 3.0+ its replacement (limitTemperature) at the moment is subject to an installation bug ... (limitTemperature missed out of the fvOptions/Make/files)
/edit
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET

Last edited by derekm; April 2, 2016 at 11:45.
derekm is offline   Reply With Quote

Old   March 31, 2016, 17:37
Default fvOptions - V3.0 lots of trouble
  #2
Senior Member
 
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 13
derekm is on a distinguished road
Be aware that in the transition to v3.0 from v2.4 some fvOptions have:
changed name,
changed location,
changed syntax


e.g

fvoptions are now in the constant directory
p, li { white-space: pre-wrap; } temperatureLimitsConstraint is no longer there, its supposed to be replaced by limitTemperature ( edit it works in 3.0.1 but not in 3.0+). I dont know if thats the only one


the location in the syntax of "selectionmode" and other stuff has changed

from
Code:
porousToair
{
    type            constantHeatTransfer;
    active          on;
    selectionMode   mapRegion;
    interpolationMethod cellVolumeWeight;
    nbrRegionName   air;
    master          true;

    constantHeatTransferCoeffs
    {
        nbrModelName    airToporous;
        fieldNames      (h);
        semiImplicit    no;
    }
}
to





Code:
porousToair
{
    type            constantHeatTransfer;
    active          yes;

    constantHeatTransferCoeffs
    {
        interpolationMethod cellVolumeWeight;
        nbrRegionName   air;
        master          true;

        nbrModelName    airToporous;
        fieldNames      (h);
        semiImplicit    no;
    }
}
can someone point me to the release notes where this was advertised as happening.
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET

Last edited by derekm; April 2, 2016 at 11:14.
derekm is offline   Reply With Quote

Old   April 2, 2016, 18:12
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Greetings Derek,

The release notes that relate to this should be the ones from OpenFOAM 3.0.0: http://www.openfoam.org/version3.0.0/ - section "Sources and Constraints (fvOptions)"

Unfortunately, there were several more changes that weren't listed in the release notes and that you've stumbled upon. These changes are listed here:
There are a couple more features I managed to list here: http://www.cfd-online.com/Forums/ope...m-3-0-0-a.html - post #2, but it's still far from listing all changes that were made.

The code present in OpenFOAM 3.0.0 was started in December 2014 and was released almost a year later, which is why the release notes are not 100% complete.


Either way, the trick in these situations is to compare a tutorial in each version of OpenFOAM to see what changed between versions for the particular feature you're trying to use.


For the record, I noticed that you've also reported a bug for this in OpenFOAM+ at https://develop.openfoam.com - in issue #89. I only haven't given a full link, given that the access is visible only to registered users on their system.

Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   April 2, 2016, 18:45
Default
  #4
Senior Member
 
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 172
Rep Power: 13
derekm is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Greetings Derek,
...

Either way, the trick in these situations is to compare a tutorial in each version of OpenFOAM to see what changed between versions for the particular feature you're trying to use.
...

Best regards,
Bruno
Normally true
alas the feature in question and its replacement donít have a presence in the tutorials
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET
derekm is offline   Reply With Quote

Old   April 2, 2016, 18:51
Default
  #5
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,975
Blog Entries: 45
Rep Power: 128
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Sorry, I saw on the second commit that I listed above, near the end, how it had changed for the other tutorials, but I forgot to look for examples for this particular fvOption
wyldckat is offline   Reply With Quote

Old   April 14, 2016, 23:20
Default
  #6
aee
Member
 
Andrew Eisenhawer
Join Date: Nov 2012
Location: Alberta, Canada
Posts: 35
Rep Power: 13
aee is on a distinguished road
So it's not just me...
Thanks for brining this up for the rest of us. I'm dealing with temperature runaway in reactingParcelFilmFoam and your info may put an end to many many hours of frustration and angst.

Thanks again!

This is what i have in fvOptions now, and it seems to be working:
temperatureLimit
{
type limitTemperature;

active true;
limitTemperatureCoeffs
{
selectionMode all;
Tmax 410;
Tmin 200.0;
}
}
The big question however, is "Is this the only way to deal with temperature runaway, or is there something that can prevent it with htcConv settings or solver parameters?"
aee is offline   Reply With Quote

Old   February 1, 2021, 01:16
Default Sidenote for OpenFOAM8
  #7
New Member
 
Fritz Nieborowski
Join Date: Nov 2020
Posts: 2
Rep Power: 0
fritznieb is on a distinguished road
I just Had similar issues as people in this thread, but seems like the Format changed so in case someone after 2020 using OpenFOAM8 has similar issues, this is my code for the system/fvOptions File that seemingly solved this issue for me.
HTML Code:
FoamFile

{
    version 2.0;
    class dictionary;
    location "system";
    format ascii;
    object fvOptions;
}
limitTemperature
{
    type limitTemperature;
    active      true;
    limitTemperatureCoeffs
    {
        selectionMode all;
        min     200;
        max     400;
    }
}

fritznieb is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Can I use fvOptions to couple a solid region and a fluid region? titanchao OpenFOAM Running, Solving & CFD 4 January 14, 2022 07:55
How to set fvOptions yurifrey OpenFOAM Pre-Processing 5 February 22, 2016 18:14
problem with fvOptions in twophase eulerfoam Hamzeh_Mirab OpenFOAM Running, Solving & CFD 0 January 27, 2015 11:04
[swak4Foam] Setting BC for a passive scalar (groovy vs fvOptions) Tobi OpenFOAM Community Contributions 0 May 23, 2013 14:53
Help required on working of Micro-oven aero CFX 4 January 19, 2007 08:21


All times are GMT -4. The time now is 05:27.