[swak4Foam] GroovyBC with power input (heat flux)

Tobi · March 9, 2015, 11:08

Hi all,

I did not get the point to build a heat flux bc with groovy.
Why I use groovy is due to the fact that I also have to use some gaussian probability distribution.

At least I used this summary: http://www.modlab.lv/docs/2011/OpenF...Vilums_pdf.pdf

So what we get is the following situation:

$T_f = f \cdot valueFraction + (1-f) \cdot (T_{centre} + gradExpr \cdot \delta)$

f is the fractionExpression.

Now I want to use the gradient expression to evaluate the temperature at the face. We get the following expression:

$\nabla T = \frac{q}{A} \cdot \frac{1}{kappa}$

This is exactly the same expression like in the turbulentHeatFluxTemperature BoundaryCondition.

Now I expect, that the fractionExpression is zero. Therefore only the second term in the first eqn. is valid and we can write:

$T_f = T_{centre} + gradExpr \cdot \delta$

This is equal to:

$\frac{T_f - T_{centre}}{\delta} = gradExpr$

and that is equal to:

$\nabla T = \frac{q}{A} \cdot \frac{1}{kappa}$

In groovyBC I used the following code:

Code:

    top
    {

        type            groovyBC;
        variables       "Kappa=160;Q=10000;g=Q/sum(mag(Sf()))/Kappa;";
        fractionExpression "0";
        gradientExpression "g";
        value           uniform 300;
    }

If I run the simulation I will get a Temperature at the faces equal to zero and I do not know why? I think I made a stupid mistake. Any suggestion is appreciated.

Thanks in advance,

zfaraday · March 9, 2015, 12:31

Hi Tobi!

Quote:

Originally Posted by Tobi

In groovyBC I used the following code:

Code:

    top
    {

        type            groovyBC;
        variables       "Kappa=160;Q=10000;g=Q/sum(mag(Sf()))/Kappa;";
        fractionExpression "0";
        gradientExpression "g";
        value           uniform 300;
    }

I haven't checked it much deeply, but with a slight glance I don't know if it's correct your definition of g. Maybe trying with this other g could solve it:

Code:

g=Q/mag(Sf())/Kappa

Let us know if it does the trick!

Btw, is the same mag(Sf()) than area()? Or does area() take the sign of normal direction into account?

Best regards,

Alex

Tobi · March 9, 2015, 14:43

Hi Alex,

I need the whole area of the surface (not only one face). If I use yours, then the heatflux will increase extreamly (dividing by a very small number).

That is not the problem.

zfaraday · March 9, 2015, 15:03

Quote:

Originally Posted by Tobi

Hi Alex,

I need the whole area of the surface (not only one face). If I use yours, then the heatflux will increase extreamly (dividing by a very small number).

That is not the problem.

Yes, you are right Tobi, sorry, I wrote that after a quick glance to the formulation without checking the calculation on paper. I got confused because recently I have been using groovyBC aswell but in my case it was for convection heat transfer not fixed power and I worked with heat fluxes instead of total heat. That's why understood wrong your formulation, I didn't remember any sum(...) below the fraction. After checking deeper your formulation, it seems to be ok... Have you managed to solve the problem with temperatures?

Tobi · March 10, 2015, 03:57

Hi,

today it is working! I don't know what was the problem. The only thing that I changed today was to set the fractionExpression to zero but if I check the first post, I already did this yesterday. Don't know but its working proper now

To your question ... area() - never used this option in groovy. Is it really a groovyBC function? It is definitly not the same as above.

Kanarya · January 12, 2016, 05:49

Dear Tobi,

I would like to use groovyBC in order to apply constant 400 kW/m^2 heat flux at the wall but I could not find how?
can you help me?
I am using OF version 2.3.1
Thanks!

Quote:

Originally Posted by Tobi

Hi,

today it is working! I don't know what was the problem. The only thing that I changed today was to set the fractionExpression to zero but if I check the first post, I already did this yesterday. Don't know but its working proper now

To your question ... area() - never used this option in groovy. Is it really a groovyBC function? It is definitly not the same as above.

Tobi · January 12, 2016, 06:17

Hi,

I think you can use "turbulentlHeatTransferTemperature" for that. You can apply the flux [W/m^2]. There is no need for groovy. If you want to use groovy you have to derive the equation yourself / or just check the pdf in the first link. It shoud be sufficient.

Kanarya · January 12, 2016, 07:07

thanks for the quick answer...yes you are right!I thought so as well but I have laminar flow so I do not have "alphaEff" so it gives me a problem

Code:

--> FOAM FATAL ERROR: 

    request for volScalarField alphaEff from objectRegistry region0 failed
    available objects of type volScalarField are

24
(
alpha.water_0
cp
alpha.vapour
interfaceProperties:K
pSat
alpha.water
mCond
kappa
rho
mVap
p_rgh
nu
gh
nu1
((hEvap*(mCond+mVap))|T)
IF
p
rho_0
nu2
T
rhoCp_0
(-IF*SLarge)
rhoCp
((IF*SLarge)*TSat)
)


    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /usr/local/OpenFOAM//OpenFOAM-2.3.1/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/usr/local/OpenFOAM//OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::error::abort() in "/usr/local/OpenFOAM//OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const in "/home/links/rek209/OpenFOAM/rek209-2.3.1/platforms/linux64GccDPOpt/lib/libphaseChangeTwoPhaseMixturesInterEvapCondPhaseChangeFoam.so"
#3  Foam::incompressible::turbulentHeatFluxTemperatureFvPatchScalarField::updateCoeffs() in "/usr/local/OpenFOAM//OpenFOAM-2.3.1/platforms/linux64GccDPOpt/lib/libincompressibleTurbulenceModel.so"
#4  Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::updateCoeffs() at /usr/local/OpenFOAM//OpenFOAM-2.3.1/src/OpenFOAM/lnInclude/PtrListI.H:36
#5  Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) at /usr/local/OpenFOAM//OpenFOAM-2.3.1/src/finiteVolume/lnInclude/fvMatrix.C:325
#6  Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::Sp<double>(Foam::DimensionedField<double, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at /usr/local/OpenFOAM//OpenFOAM-2.3.1/src/OpenFOAM/lnInclude/tmpI.H:191
#7  Foam::tmp<Foam::fvMatrix<double> > Foam::fvm::Sp<double>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) at /usr/local/OpenFOAM//OpenFOAM-2.3.1/src/OpenFOAM/lnInclude/tmpI.H:176
#8  
 at /scratch/rkahraman/evapCond/interEvapCondPhaseChangeFoam_allfiles/interExCondPhaseChangeFoam/TEqn.H:36
#9  __libc_start_main in "/lib64/libc.so.6"
#10  
 in "/home/links/rek209/OpenFOAM/rek209-2.3.1/platforms/linux64GccDPOpt/bin/interExCondPhaseChangeFoam"
Aborted

Quote:

Originally Posted by Tobi

Hi,

I think you can use "wallHeatTransfer" for that. You apply Tinf and alpha there. There is no need for groovy. If you want to use groovy you have to derive the equation that have to be implemented in groovy yourself / or just check the pdf in the first link.

Thanks for your help

Tobi · January 12, 2016, 07:15

Hi,

it seems that its your own solver. Do you have a field implemented that correspond to "thermal diffusivity"? If yes then use that, otherwise implement it to your solver or change the BC or if you want, use groovy.

Kanarya · January 12, 2016, 09:37

Thanks again...the problem is I know only the thermal conductivity and heat flux, so I can not implement groovyBC...do you have any idea how i can build the groovyBC in order to have fix heat flux?

BEST!

Tobi · January 12, 2016, 10:04

Hi,

I don't know what your application is for and what you actually want to do but if I understand it correct you can use the groovy in the first post:

March 9, 2015, 11:08	GroovyBC with power input (heat flux)	#1
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi all, I did not get the point to build a heat flux bc with groovy. Why I use groovy is due to the fact that I also have to use some gaussian probability distribution. At least I used this summary: http://www.modlab.lv/docs/2011/OpenF...Vilums_pdf.pdf So what we get is the following situation: $T_f = f \cdot valueFraction + (1-f) \cdot (T_{centre} + gradExpr \cdot \delta)$ f is the fractionExpression. Now I want to use the gradient expression to evaluate the temperature at the face. We get the following expression: $\nabla T = \frac{q}{A} \cdot \frac{1}{kappa}$ This is exactly the same expression like in the turbulentHeatFluxTemperature BoundaryCondition. Now I expect, that the fractionExpression is zero. Therefore only the second term in the first eqn. is valid and we can write: $T_f = T_{centre} + gradExpr \cdot \delta$ This is equal to: $\frac{T_f - T_{centre}}{\delta} = gradExpr$ and that is equal to: $\nabla T = \frac{q}{A} \cdot \frac{1}{kappa}$ In groovyBC I used the following code: Code: top { type groovyBC; variables "Kappa=160;Q=10000;g=Q/sum(mag(Sf()))/Kappa;"; fractionExpression "0"; gradientExpression "g"; value uniform 300; } If I run the simulation I will get a Temperature at the faces equal to zero and I do not know why? I think I made a stupid mistake. Any suggestion is appreciated. Thanks in advance, Kanarya and Marpole like this. __________________ Keep foaming, Tobias Holzmann

January 12, 2016, 10:04		#11
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi, I don't know what your application is for and what you actually want to do but if I understand it correct you can use the groovy in the first post: __________________ Keep foaming, Tobias Holzmann

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Conjugate Heat Transfer: Wall Heat Flux at Coupled Walls?	MaxHeat	FLUENT	4	September 14, 2017 10:44
Forced convective heat transfere with fixed heat flux?	BenFranklinIII	OpenFOAM Running, Solving & CFD	0	July 30, 2015 05:31
[OpenFOAM] Paraview 3.98 - errors when saving geometry file	pajot	ParaView	1	September 28, 2013 10:45
Heat Flux Profile at Fluid-Porous Interface	Hitch8	CFX	4	December 15, 2012 09:57
groovyBC nonuniform Wall heat flux	Shoonya	Main CFD Forum	0	August 11, 2010 13:03

March 9, 2015, 14:43		#3
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi Alex, I need the whole area of the surface (not only one face). If I use yours, then the heatflux will increase extreamly (dividing by a very small number). That is not the problem. __________________ Keep foaming, Tobias Holzmann

March 10, 2015, 03:57		#5
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi, today it is working! I don't know what was the problem. The only thing that I changed today was to set the fractionExpression to zero but if I check the first post, I already did this yesterday. Don't know but its working proper now To your question ... area() - never used this option in groovy. Is it really a groovyBC function? It is definitly not the same as above. __________________ Keep foaming, Tobias Holzmann

January 12, 2016, 06:17		#7
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi, I think you can use "turbulentlHeatTransferTemperature" for that. You can apply the flux [W/m^2]. There is no need for groovy. If you want to use groovy you have to derive the equation yourself / or just check the pdf in the first link. It shoud be sufficient. __________________ Keep foaming, Tobias Holzmann

January 12, 2016, 07:15		#9
Tobi Super Moderator Tobias Holzmann Join Date: Oct 2010 Location: Tussenhausen Posts: 2,708 Blog Entries: 6 Rep Power: 51	Hi, it seems that its your own solver. Do you have a field implemented that correspond to "thermal diffusivity"? If yes then use that, otherwise implement it to your solver or change the BC or if you want, use groovy. __________________ Keep foaming, Tobias Holzmann

January 12, 2016, 09:37		#10
Kanarya Senior Member Join Date: May 2011 Posts: 231 Rep Power: 15	Thanks again...the problem is I know only the thermal conductivity and heat flux, so I can not implement groovyBC...do you have any idea how i can build the groovyBC in order to have fix heat flux? BEST!