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

twoPhaseEulerFoam + fvOptions limitTemperature

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

Like Tree2Likes
  • 2 Post By hanness

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 4, 2016, 03:18
Default twoPhaseEulerFoam + fvOptions limitTemperature
  #1
Member
 
hannes
Join Date: Mar 2013
Posts: 47
Rep Power: 13
hanness is on a distinguished road
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;
                }

}
but the simulation won't start with the following error report:
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)
I can't find a way to restrict the fvOptions file to just one phase nor can I find a hint in the source code, that it is actually usable with multiphase solvers. Does anybody have any idea?

Thanks a lot
Hannes
FlyFox and rasool_soofi like this.
hanness is offline   Reply With Quote

Old   July 1, 2016, 10:34
Default
  #2
Member
 
Sebastian W.
Join Date: Nov 2012
Location: Saxony, Germany
Posts: 43
Rep Power: 13
nero235 is on a distinguished road
Send a message via ICQ to nero235
Quote:
Originally Posted by hanness View Post
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;
                }

}
but the simulation won't start with the following error report:
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)
I can't find a way to restrict the fvOptions file to just one phase nor can I find a hint in the source code, that it is actually usable with multiphase solvers. Does anybody have any idea?

Thanks a lot
Hannes
Hey there,

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
nero235 is offline   Reply With Quote

Old   July 26, 2016, 08:44
Default
  #3
New Member
 
Join Date: Jan 2016
Posts: 10
Rep Power: 10
katete is on a distinguished road
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;
        }
        
}
So maybe you have to define the selection mode as well: selectionMode all;

Hope this helps.
Best regards
Katharina
katete is offline   Reply With Quote

Old   August 18, 2016, 02:53
Default
  #4
Member
 
Kumar
Join Date: Jun 2013
Posts: 47
Rep Power: 13
kishpishar is on a distinguished road
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
kishpishar is offline   Reply With Quote

Old   February 27, 2018, 05:01
Default
  #5
New Member
 
Jose Rothkegel
Join Date: Mar 2015
Posts: 7
Rep Power: 11
FlyFox is on a distinguished road
Quote:
Originally Posted by hanness View Post
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;
                }

}
but the simulation won't start with the following error report:
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)
I can't find a way to restrict the fvOptions file to just one phase nor can I find a hint in the source code, that it is actually usable with multiphase solvers. Does anybody have any idea?

Thanks a lot
Hannes
Hello,
Did you finally solve this issue?
FlyFox is offline   Reply With Quote

Old   July 19, 2018, 08:53
Default
  #6
Member
 
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 11
Robin.Kamenicky is on a distinguished road
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
     }
I have tested that at reactingTwoPhaseEulerFoam.

Cheers,
Robin
Robin.Kamenicky 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
fvOptions: temperatureLimitsConstraint or limitTemperature not working on V3.0+ derekm OpenFOAM Running, Solving & CFD 6 February 1, 2021 01:16
fvOptions with twoPhaseEulerFoam: momentumSource rdbisme OpenFOAM Pre-Processing 2 March 21, 2016 05:39
twoPhaseEulerFoam fvOptions for alpha lavdwall OpenFOAM Running, Solving & CFD 8 October 19, 2015 09:57
Is twoPhaseEulerFoam applicable to 3D cases / delivering erroneous results? ThomasV OpenFOAM 0 November 11, 2013 08:10


All times are GMT -4. The time now is 06:09.