|
[Sponsors] |
twoPhaseEulerFoam + fvOptions limitTemperature |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 4, 2016, 04:18 |
twoPhaseEulerFoam + fvOptions limitTemperature
|
#1 |
Member
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 13 |
Hi all,
is there a way to use limitTemperature with twoPhaseEulerFoam in OF301? my constant/fvoptions looks as following: Code:
valueLimitation { type limitTemperature; active true; limitTemperatureCoeffs { selectionMode all; Tmin 50; Tmax 150; } } Code:
Selecting finite volume options model type limitTemperature Source: valueLimitation - selecting all cells - selected 46875 cell(s) with volume 0.0225 --> FOAM FATAL ERROR: request for basicThermo thermophysicalProperties from objectRegistry region0 failed available objects of type basicThermo are 2 ( thermophysicalProperties.air thermophysicalProperties.water ) From function objectRegistry::lookupObject<Type>(const word&) const in file /opt/openfoam30/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) at ??:? #1 Foam::error::abort() at ??:? #2 Foam::basicThermo const& Foam::objectRegistry::lookupObject<Foam::basicThermo>(Foam::word const&) const at ??:? #3 Foam::fv::limitTemperature::limitTemperature(Foam::word const&, Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&) at ??:? #4 Foam::fv::option::adddictionaryConstructorToTable<Foam::fv::limitTemperature>::New(Foam::word const&, Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&) at ??:? #5 Foam::fv::option::New(Foam::word const&, Foam::dictionary const&, Foam::fvMesh const&) at ??:? #6 Foam::fv::optionList::reset(Foam::dictionary const&) at ??:? #7 Foam::fv::optionList::optionList(Foam::fvMesh const&, Foam::dictionary const&) at ??:? #8 Foam::fv::IOoptionList::IOoptionList(Foam::fvMesh const&) at ??:? #9 ? at ??:? #10 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6" #11 ? at ??:? Aborted (core dumped) Thanks a lot Hannes |
|
July 1, 2016, 11:34 |
|
#2 | |
Member
|
Quote:
I have a similar problem running twoPhaseEulerFoam coupled with a source in the fvOptions file. Have you found a solution to the problem? Regards, Sebastian |
||
July 26, 2016, 09:44 |
|
#3 |
New Member
Join Date: Jan 2016
Posts: 10
Rep Power: 10 |
Hey,
for OF 2.4.0 this definition worked for me: Code:
temperature_constraints { type temperatureLimitsConstraint; selectionMode all; active true; temperatureLimitsConstraintCoeffs { Tmin 299; Tmax 300; } } Hope this helps. Best regards Katharina |
|
August 18, 2016, 03:53 |
|
#4 |
Member
Kumar
Join Date: Jun 2013
Posts: 47
Rep Power: 13 |
Hi Sebastian,
Have you found out a way to use the limitTemperature in twoPhaseEulerFoam in OF-3.0.1? I have the same problem. As Katharina said, the equivalent temperatureLimitsConstraint works perfectly for me in OF-2.3.1 Thanks Kumar |
|
February 27, 2018, 06:01 |
|
#5 | |
New Member
Jose Rothkegel
Join Date: Mar 2015
Posts: 7
Rep Power: 11 |
Quote:
Did you finally solve this issue? |
||
July 19, 2018, 09:53 |
|
#6 |
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 11 |
Hi Foamers,
Despite the old thread, I would like to mention an update. Thanks to OF developers there is a new option in the new version OpenFAOM-6 to define phase for which the limiTemperature is applied. This solution seems to work well. Code:
limitT { type limitTemperature; active yes; selectionMode all; min 200; max 500; phase gas; // optional } Cheers, Robin |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 08:55 |
fvOptions: temperatureLimitsConstraint or limitTemperature not working on V3.0+ | derekm | OpenFOAM Running, Solving & CFD | 6 | February 1, 2021 02:16 |
fvOptions with twoPhaseEulerFoam: momentumSource | rdbisme | OpenFOAM Pre-Processing | 2 | March 21, 2016 06:39 |
twoPhaseEulerFoam fvOptions for alpha | lavdwall | OpenFOAM Running, Solving & CFD | 8 | October 19, 2015 10:57 |
Is twoPhaseEulerFoam applicable to 3D cases / delivering erroneous results? | ThomasV | OpenFOAM | 0 | November 11, 2013 09:10 |