[jvinuales]

Hi everyone,

I am using OpenFOAM v2006. I use a modified version of buoyantBoussinesqSimpleFoam (removing buoyant effects) in order to study forced convetion on internal flows.

I want to use limitTemperaure option in fvOptions but I got an error about thermophysicalProperties, as these are not utilised in buoyantBoussinesqSimpleFoam (I tried to add them in constant but does not work)

request for basicThermo thermophysicalProperties from objectRegistry region0 failed
    available objects of type basicThermo are
0()

Is there a way I can use this option at all with this solver?

Thanks.

[jvinuales]

Or any other alternatives to use temperature limiters?

[jvinuales]

anyone has a clue?

[HPE]

Hi,

is there any way to test a tutorial, so that we can replicate the issue of yours locally? And then potentially, find a solution.

To my knowledge, there is no other temperature limiter fvOption available in OpenFOAM.

[jvinuales]

Sure thing, thanks for your reply. In order to recreate the error easily, I just added the fvOptions to the iglooWithFridges tutorial (buoyantBoussinesqSimpleFoam solver):

fvOptions:

limitT
{
    type       		limitTemperature;
    min        		0;
    max        		2000;
    selectionMode 	all;
	active      	yes;
}

error:

Selecting finite volume options type limitTemperature
    Source: limitT
    - selecting all cells
    - selected 7197 cell(s) with volume 129.524


--> FOAM FATAL ERROR: 

    request for basicThermo thermophysicalProperties from objectRegistry region0 failed
    available objects of type basicThermo are
0()

    From const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::basicThermo]
    in file /home/pawan/OpenFOAM/OpenFOAM-v2006/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 463.

[jherb]

You are right, the existing limitTemperatue fvOption does not work with buoyantBoussinesqSimple/PimpleFoam solvers. You have to implement them yourself.
You can do this by copying the existing one, giving it a new name and compile it into seperate library. I think, the only thing you need to change is this line: https://github.com/OpenFOAM/OpenFOAM...tTemperature.C

fieldNames_.setSize(1, thermo.he().name());

into

fieldNames_.setSize(1, "T");

[shock77]

Hi,


I have had the more or less the same issue when I wanted to use limitTemperature with rhoCentralFoam. I have implemented it myself, which is described in this thread: Sudden Increase of residuals.


I am using openfoam4.

[jvinuales]

Thanks both for your answers. I will try to modify the existing limitTemperature as suggested by Joachim. Do you have any guidance about how to compile a new library? So far, I just have compiled new solvers, which is more straighforward.

[jherb]

These links should help (even if the first two are about a new boundary condtions instead of fvOptions):


https://openfoamwiki.net/index.php/H...dary_condition
https://www.youtube.com/watch?v=t0Vj2O_9HBQ
http://www.tfd.chalmers.se/~hani/kur..._Segersson.pdf

[SHUBHAM9595]

As mentioned here fvOptions: temperatureLimitsConstraint or limitTemperature not working on V3.0+ if u r using recent versions then this issue might be fixed already.....

However, if u r old school and still using former versions (like me)....Here's the attached file that have all the necessary modifications required to limit the Temperature......

Thanks to Joachim for the hint limitTemperature in buoyantBoussinesqSimpleFoam

However only commenting out that part wont solve the problem............The issue seems to arise bcz of the 'he' (either enthalpy or specific internal energy)based formulation of the Energy equation....thus the inherent version will try to limit "he" instead of directly putting constraints on T......

1)Extract the zip file,move its contents to $FOAM_SRC/fvOptions/corrections/customLimitTemp
2)Dont forget to update fvoptions/Make/file to

/* Corrections */

corrections/limitTemperature/limitTemperature.C
corrections/limitVelocity/limitVelocity.C
corrections/customLimitTemp/customLimitTemp.C


LIB = $(FOAM_USER_LIBBIN)/libfvOptions

3) wclean libso followed by wmake libso...........and u r good to go