heat transfer with OpenFoam
 

Dear all,

I want to model a turbulent flow with heat transfer caused by forced convection and radiation.
How can I model that with OF. I have checked the tutorial files of the heat transfer solvers. I every solver-file there are the following files: alphatwallfunction, epsilon, k, nut, p, p_rgh, T, T.org, U.
- What is the meaning of them (T=temperature, U=velocity.)?
- Is it possible to enter a heat transfer coefficient calculated by my own or does OF calculate everything by itself?

Thank you for your answer.

Best Regards,
tH3f0rC3

hi,
may be this will help you:
-alphatWallFunction=turbulent thermal diffusity (or eddy thermal diffusity)
-k=turbulent energy
-epsilon=dissipation
-nut=turbulent viscosity
-p=pressure, exact: pressure/rho for inkompressible Solver
-p_rgh=hydrostatic pressure p_0+rho*g*h (same as above p_0/rho+g*h); if g=(0 0 0) than p=p_rgh
-T=temperature [K]
-T.org=backup for T
-U=velocity (vector)
and the last, which you forget
-kappat=turbulent thermal conductivity

i think you define the heat transfer coefficient over the Pr in transportProperties. but i'm not sure.

Thank you for your answer!

I have now checked the buoyantSimpleRadiationFoam-solver. There are some more files.
Do you know the meaning of them, too?

G
mut

Regards,
tH3f0rC3

I have tried to use the buoyantSimpleRadiationFoam-solver for an easy model.
The folliwing error appears:

Create time
Create mesh for time = 0

Reading g
Reading thermophysical properties
Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThe rmo<hConstThermo<perfectGas>>>>>
#0 Foam::error::printStack(Foam::Ostream&) in "/data/caehgb.za/studienarbeit-di rk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOA M.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/data/caehgb.za/studienarbeit-dirk/work /OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt in "/lib64/tls/libc.so.6"
#3 Foam::hPsiThermo<Foam::pureMixture<Foam::constTran sport<Foam::specieThermo<F oam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/data/caehgb.za/stu dienarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPO pt/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::constTran sport<Foam::specieThermo<F oam::hConstThermo<Foam::perfectGas> > > > >::hPsiThermo(Foam::fvMesh const&) in "/data/caehgb.za/studienarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7 .1/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#5 Foam::basicPsiThermo::addfvMeshConstructorToTable< Foam::hPsiThermo<Foam::pur eMixture<Foam::constTransport<Foam::specieThermo<F oam::hConstThermo<Foam::perfec tGas> > > > > >::New(Foam::fvMesh const&) in "/data/caehgb.za/studienarbeit-dirk /work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libbasicTher mophysicalModels.so"
#6 Foam::basicPsiThermo::New(Foam::fvMesh const&) in "/data/caehgb.za/studienar beit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/lib basicThermophysicalModels.so"
#7 main in "/data/caehgb.za/studienarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/ OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/buoyantSimpleRadiationFoam"
#8 __libc_start_main in "/lib64/tls/libc.so.6"
#9 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream: :versionNumber, Foam::IOstream::compressionType) const in "/data/caehgb.za/studi enarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/applications/bin/li nux64GccDPOpt/buoyantSimpleRadiationFoam"
Floating point exception

Can someone help me?
Maybe OF isn't installed correct?

Regards

Hi ang_dipl_ing_fd,

do you also know the following:
In the thermophysical properties:
mixture air 1 28.9 1000 0 1.8e-05 0.7;

What does that mean?
Does every number have a meaning?

Best Regards

Hi

In the thermophysical properties:
mixture air 1 28.9 1000 0 1.8e-05 0.7;

The thermalPhsical Properties is calculated based which model you specified, like
if model is hPsiThermo, calculation based on enthalpy 'h' and compressibility 'psi'.
and if model is hRhoThermo, calculation based on enthalpy or sensible enthalpy.
and if model is pureMixture, calculation based on passive gas mixtures.

parameters :

air is mixture fluid name
1 is for pure Mixture (mixture property) (number of molecules of species)
28.9 for molecule weight (kg/kmol)
1000 for heat capacity at constant pressure [J/kmol K]
0 for reference enthalpy [J/kmol]
1.8e-05 for Dynamics viscosity (kg/ms)
0.7 is for Prandtl number.

you can change properties according to your problem (fluid).

best luck

Alpesh

Hi tH3f0rc3 (hard to say :-p)

As far as I know:

1 => Number of moles of this specie
28,9 => Molecular weight
1000 => Cp (Specific heat capacity)
0 => heat of fusion (useless, I guess in your case)
1.8e-05 => dynamic viscosity
0.7 => Prantl number

I'm also interested in this matter (I've got the same issue but with chtMultiRegionSimpleFoam). Someone clever than us? ^^

Cheers guys :)

[Edit]: I was too slow, apparently (damn coffee break ! :-D), sorry for this double answer

Hey,
thanks for your answer.
Do you also know, where I can type in the properties of the walls, for example that a wall consists of nickel?

Regards,
tH3f0rC3

OK, but I think i have to gibe the solver an information of the material which should be heaten up. For example the density or cp...
Where can I do that?

Best Regards,
tH3f0rC3

I think I got your case wrong:
Can you explain briefly what your heat transfer consist in? And add your directories files also, if you don't mind.

I want to simulate a heat transfer from a turbulent (I guess so) flow to a surface, that should be heaten up.
In addition to that there is also radiation from the hot wall to the surface.

If this description is too short, please let me know.

Which files do you want to see?

Regards,
tH3f0rC3

Hi sixwp,

it is exactly the same issue just with other file dorectory?

Regards

I'm sorry, I must be tired, I don't really see what's your geometry's like. Can you show me a raw scheme?

Concerning the directories files: can you post your 0, constant and system folders? Maybe (not likely but, who knows), I'll be able to find out your problem and therefore, mine :-)

Yes, of course.
But you have to give me an email adress of yours, because I can't post fotos.

Regards

Hi,

is there someone else, who understands the following error message?

Create time
Create mesh for time = 0

Reading g
Reading thermophysical properties
Selecting thermodynamics package hPsiThermo<pureMixture<constTransport<specieThe rmo<hConstThermo<perfectGas>>>>>
#0 Foam::error::printStack(Foam::Ostream&) in "/data/caehgb.za/studienarbeit-di rk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOA M.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/data/caehgb.za/studienarbeit-dirk/work /OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 __restore_rt in "/lib64/tls/libc.so.6"
#3 Foam::hPsiThermo<Foam::pureMixture<Foam::constTran sport<Foam::specieThermo<F oam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/data/caehgb.za/stu dienarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPO pt/libbasicThermophysicalModels.so"
#4 Foam::hPsiThermo<Foam::pureMixture<Foam::constTran sport<Foam::specieThermo<F oam::hConstThermo<Foam::perfectGas> > > > >::hPsiThermo(Foam::fvMesh const&) in "/data/caehgb.za/studienarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7 .1/lib/linux64GccDPOpt/libbasicThermophysicalModels.so"
#5 Foam::basicPsiThermo::addfvMeshConstructorToTable< Foam::hPsiThermo<Foam::pur eMixture<Foam::constTransport<Foam::specieThermo<F oam::hConstThermo<Foam::perfec tGas> > > > > >::New(Foam::fvMesh const&) in "/data/caehgb.za/studienarbeit-dirk /work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libbasicTher mophysicalModels.so"
#6 Foam::basicPsiThermo::New(Foam::fvMesh const&) in "/data/caehgb.za/studienar beit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/lib basicThermophysicalModels.so"
#7 main in "/data/caehgb.za/studienarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/ OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/buoyantSimpleRadiationFoam"
#8 __libc_start_main in "/lib64/tls/libc.so.6"
#9 Foam::regIOobject::writeObject(Foam::IOstream::str eamFormat, Foam::IOstream: :versionNumber, Foam::IOstream::compressionType) const in "/data/caehgb.za/studi enarbeit-dirk/work/OpenFoam_ParaView/OpenFOAM/OpenFOAM-1.7.1/applications/bin/li nux64GccDPOpt/buoyantSimpleRadiationFoam"
Floating point exception

I know now, that this error message appears every time I want to involve the heat transfer.
Maybe this helps.

hi tH3f0rC3,
did you run the tutorials without any change?

Hi,

if I get you right you just have one fluid domain.
If you want to know the interaction of the fluid with a connected solid than you need a multiregion solver.
(density and cp are values connected to a volume and not to a surface)

Regards,
Toni

Hello,

I have another question to
-k=turbulent energy
-epsilon=dissipation
-nut=turbulent viscosity

I have to set up these files in the 0-file as boundary cinditions.
k and epsilon must have a value for the inlet surfaces. But how can I calculate these values?
And what is meant with the values

Hello,

I have another question to
-k=turbulent energy
-epsilon=dissipation
-nut=turbulent viscosity

I have to set up these files in the 0-file as boundary cinditions.
k and epsilon must have a value for the inlet surfaces. But how can I calculate these values?
And what is meant with the values
Cmu 0.09;
kappa 0.41;
E 9.8;
They are automatically set up as written above.

What do they mean?

Best Regards,
tH3f0rC3

hi dirk,
may be this will help you

http://www.cfd-online.com/Wiki/Turbu...ary_conditions

the other values are default model coefficients which i would not change.

Hi,

thank you, that's a very good link! :-)

In the description is written that k and epsilon must be specified for the inlet boundaries.
But how do I set up the walls or outlets?

The suggestion of ANSA is to set zeroGradient to walls and outlets. ANSA suggests this by outputting the file as an OpenFoam case. So i don't know if this is right.

Another question is how to set up inlet and outlet layers in nut. For walls I can use nutwallfunction but what shall I use for inlet and outlets.
The suggestion of ANSA in this case is also zeroGradient.

Best Regards,
tH3f0rC3

hi dirk,
i would use for k and epsilon:
...
outlet
{
type inletOutlet;
inletValue $internalField; // or you calculate with estimated values
value $internalField; // only a placeholder
}
...

and for nut:

"(inlet|outlet)" // so you specify inlet AND outlet at the same time
{
type calculated;
}

for walls you can use wall function for k and epsilon
"(wallA|wallB|wallC)"
{
type kqRWallFunction; // wall function for k, q and R
}

and

wall
{
type epsilonWallFunction;
}

This is for incompressible simulation!!!
If you are fluid is compressible than you have to set

type compressible::"Wall_Function";

I got a similar error a few days ago when solving a heat-transfer-case. I got rid of it by not setting the temperature to 0 K anywhere ;)
Maybe that helps someone...

Change pressure
 

You probably have a zero pressure at the internalField. Any how, I got the same message and it went away when I was changing the internal pressure and pressure at outlet.

Gr Peter