CFD Online Discussion Forums - buoyantBoussinesqPimpleFoam

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Pre-Processing (https://www.cfd-online.com/Forums/openfoam-pre-processing/)

- - buoyantBoussinesqPimpleFoam - Heat capacity on wall BC (https://www.cfd-online.com/Forums/openfoam-pre-processing/101702-buoyantboussinesqpimplefoam-heat-capacity-wall-bc.html)

buoyantBoussinesqPimpleFoam - Heat capacity on wall BC

Hello,
I'm working with buoyantBoussinesqPimpleFoam solver simulating the flow of water in pipes.
Is it possible to define the walls as having heat capacity ?

This could give a first approximation of how a warmer fluid is going to be cooled (and for how long) flowing in colder pipes. Without using multiple regions solvers, I mean.

Thanks,

At the moment I'm trying to use groovyBC to create a relation between the temperature of each cell on the walls to the one of closer cell (but not of the walls).

Someone could indicate whether this could be the right (approximate) approach ?

Or do I definetely need a multiregion case ?

Thanks.

I found a good BC... in CFX :(. Here enclosed you can see a picture I found on one of its paper (I hope one is allowed to reproduce them here).

The note on this picture is:

Quote:

Bulk Heat Transfer Coefficient / Heat Transfer Coefficient
Specify the heat flux at a Wall boundary implicitly using a solid side
heat transfer coefficient, hc , and an external temperature, Ts.
This boundary condition can be used to model several sources of
thermal resistance outside the computational domain. In the diagram
below, a lumped resistance consisting of the thermal resistance of an
external boundary layer and the bounding wall is modelled using a

single heat transfer coefficient and external temperature.

Tp is the temperature at the internal near-wall boundary element centre node.

I hope now it's more clear what I'd like to obtain. Is there any possibility to get the same result in OF ?
I know the answer is yes but my math capability are a little...rusty :o.

Any help ?

I'm not sure I understood your question. But if you need a BC with a heat transfer coefficient and an external temperature you already have the BC named "externalWallHeatFluxTemperature" in OF.

The input is [h & T external] OR [q] with q = h * (T external - T internal).

Thanks Aurelien, It seems what I need.

Unfortunately I don't have it as a BC choice...

Code:

 

--> FOAM FATAL IO ERROR:

Unknown patchField type externalWallHeatFluxTemperature for patch type wall

Valid patchField types are :

66

(

advective

atmBoundaryLayerInletEpsilon

buoyantPressure

calculated

codedFixedValue

codedMixed

cyclic

cyclicAMI

cyclicSlip

directionMixed

empty

epsilonWallFunction

fan

fanPressure

fixedFluxPressure

fixedGradient

fixedInternalValue

fixedPressureCompressibleDensity

fixedValue

freestream

freestreamPressure

inletOutlet

inletOutletTotalTemperature

kappatJayatillekeWallFunction

kqRWallFunction

mapped

mappedField

mappedFixedInternalValue

mappedFixedPushedInternalValue

mixed

nonuniformTransformCyclic

nutLowReWallFunction

nutTabulatedWallFunction

nutURoughWallFunction

nutUSpaldingWallFunction

nutUWallFunction

nutkAtmRoughWallFunction

nutkRoughWallFunction

nutkWallFunction

omegaWallFunction

oscillatingFixedValue

outletInlet

outletMappedUniformInlet

partialSlip

processor

processorCyclic

rotatingTotalPressure

sliced

slip

symmetryPlane

syringePressure

timeVaryingMappedFixedValue

totalPressure

totalTemperature

turbulentHeatFluxTemperature

turbulentInlet

turbulentIntensityKineticEnergyInlet

turbulentMixingLengthDissipationRateInlet

turbulentMixingLengthFrequencyInlet

uniformDensityHydrostaticPressure

uniformFixedValue

uniformTotalPressure

waveSurfacePressure

waveTransmissive

wedge

zeroGradient

)

 

file: F:/TAPS/CFD/f900buoyw/0/T::boundaryField::walls from line 41 to line 45.

    From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)

    in file /home/bmss/OpenFOAM/OpenFOAM-2.1/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 135.

FOAM exiting

I have to check whether in last releases its name has been changed. I'll post any progress.

Well, I think externalWallHeatFluxTemperature is just for compressible solvers.

Is there any way to have it using buoyantBoussinesqPimpleFoam ?

Greetings to all!

@Daniele:

Quote:

Originally Posted by danvica (Post 361017)

Well, I think externalWallHeatFluxTemperature is just for compressible solvers.

Try this:

Code:

compressible::externalWallHeatFluxTemperature

If you go to the tutorials folder and run (in MSys) this command:

Code:

grep -r 'compressible::' *

You'll see several other tutorials where this is explicitly defined.

Best regards,
Bruno

Thanks Bruno.

Unfortunately, it still returns the same errror.

BTW, my BC is:

Code:

walls

    {

        type            compressible::externalWallHeatFluxTemperature;

        Ta              uniform 300;

        h               uniform 3;           // test value

        value           uniform 300;

    }

Do I need to include some object/class ? I checked the tutorials but I wasn't able to find any info.

I think I was using this BC with a "BasicRhoThermo" for the fluid. If you are using a BasicPsiThermo it could lead to an error.

Try to use it by modifying a tutorial. If it works, you will have to change the source code or your solver.

Just a small update.
I checked what's inside externalWallHeatFluxTemperature and basically it's what I need:

Code:

00222     forAll (*this, i)

00223     {

00224         if (q[i] > 0) //in

00225         {

00226             this->refGrad()[i] = q[i]/K(*this)()[i];

00227             this->refValue()[i] = 0.0;

00228             this->valueFraction()[i] = 0.0;

00229         }

00230         else //out

00231         {

00232             this->refGrad()[i] = 0.0;

00233             this->refValue()[i] = KDelta[i]*q[i] + patchInternalField()()[i];

00234             this->valueFraction()[i] = 1.0;

00235         }

00236     }

where q is defined as q = (Ta_ - *this)*h_;

So, based on the direction of the Heat flux (q), externalWallHeatFluxTemperature sets the right BC.

In order to reproduce this behavior I used groovyBC in this way:

Code:

 

walls

    {

        type groovyBC;

        value uniform 300;

        gradientExpression "gradT";

        fractionExpression "0";

        variables "Text=300;hc=10000;gradT=(Text-T)*hc;";

        timelines ();

    }

Note:
- I'm just considering an entering flux.
- I still have to understand what physical value has hc (normally, heat transfer coefficient). In my BC it groups K too, that I think it rappresent specific heat.
- hc=10000 is just a test value.

Any comment or suggestion would be helpfull, thanks.

Hello,
I have some problem with externalWallHeatFluxTemperature which is not working properly with OF2.1.0
I can not switch to OF211 because GroovyBC is not working with this new version.

Thus, I tried to replace externalWallHeatFluxTemperature with a groovy boundary condition.

Code:

walls

    {

        type groovyBC;

        value uniform 300;

        gradientExpression "gradT";

        fractionExpression "0";

        variables "Text=300;hc=10000;gradT=(Text-T)*hc;";

        timelines ();

    }

This boundary condition seems to work, but I have to use hc=hext/lambda, and I am not sure why. Can someone explain this ?

I was also using wallexternalHF as an entering heat flux.
Could it be also done with groovyBC ?

Quote:

Originally Posted by danvica (Post 361017)

Well, I think externalWallHeatFluxTemperature is just for compressible solvers.

Is there any way to have it using buoyantBoussinesqPimpleFoam ?

Hi,

I´m having the same problem... did anyone manage to compile this for an incompressible solver?

Thanks,

Paula