[mabinty]

Originally Posted by murrdpirate

Thanks. I didn't realize there were examples in the code for these things.

Issue now is that it's saying "KName is undefined." As you showed, that's not listed in the example. I see somewhere online that it's "CHARACTER*(*) array of species names," but I don't know what that means

It would be easier to figure out the problem if we can see the exact error message! Try to add the line:

KName          K;

Check src/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/temperatureCoupledBase/temperatureCoupledBase.C to see what is happening with "KName".

Cheers,
Aram

[murrdpirate]

Here's the error I get when KName isn't defined:

--> FOAM FATAL IO ERROR:
keyword KName is undefined in dictionary "/home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0/T::boundaryField::window"

file: /home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0/T::boundaryField::window from line 44 to line 49.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 400.

FOAM exiting

Your suggestion to add "KName K;" made sense and actually did allow my case to calculate as normal, but for some reason I get the following error when I try to view the data in paraView (I also get the same error when running reconstructPar if I calculated in parallel):

--> FOAM FATAL IO ERROR:

Cannot find 'value' entry on patch walls of field T in file "/home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0.0005/T"
which is required to set the values of the generic patch field.
(Actual type compressible::turbulentHeatFluxTemperature)

Please add the 'value' entry to the write function of the user-defined boundary-condition


file: /home/kevin/OpenFOAM/kevin-2.0.0/run/dormCool/0.0005/T::boundaryField::walls from line 77556 to line 83919.

From function genericFvPatchField<Type>::genericFvPatchField(con st fvPatch&, const Field<Type>&, const dictionary&)
in file genericFvPatchField/genericFvPatchField.C at line 71.

FOAM exiting

Again, thanks for the help, I do feel like I'm at least getting there. I'll look into this a little bit more tonight when I have time and share what I find.

[pitmanm]

I can confirm that this error occurs also when attempting to recomposePar a model that makes use of turbulentHeatFluxTemperature boundary condition.

It appears to be a bug in the turbulentHeatFluxTemperature boundary condition in OpenFOAM 2.0 where this BC does not write the "value" entry for this BC. A look at the code seems to confirm this.

I am thinking of copying the BC to create a user-defined boundary condition which fixes the problem of writing the 'value' entry. Does anyone else know of a fix or workaround that I may not have considered?

[mauro.p.arruda@gmail.com]

hi pitmanm,

have you been able to get around the bug?

Get the same problem when converting the time directories for post-processing.

I just started looking into it and will let you know if i'm lucky or not

Cheers,

Mauro

[pitmanm]

Hi Mauro,

I have not had a chance as of yet because I've been so busy with work. The change in the code is pretty easy it is just actually just getting the fvPatchScalarField to work as a user-defined BC I have found tricky. Do you need to do it all as template classes? Then just define <scalar> perhaps?

Cheers,

Mark

[jaromin]

Hi,

"The problem is that the postprocessing utilities do not know about that b.c. so do not know how to read it (it is derived from a fixedGradient b.c. which does not need a 'value' field).

If you add the library that contains the compressible::turbulentHeatFluxTemperature to your 'libs' section in the system/controlDict it should work.

libs ("libcompressibleTurbulenceModel.so"); "

see: http://www.openfoam.com/mantisbt/view.php?id=285

Maria

[socrates]

I am trying to apply a constant BC on micro-tubes surfaces inside a substrate. I have tried these:
1.

{
type fixedGradient;
gradient uniform -10000;
}

2.

{
type groovyBC;
gradientExpression "-10000";
fractionExpression "0";
}

3.

{
type groovyBC;
value uniform 300;
gradientExpression "gradT";
variables "htot=15000.00;Tinf=293.00;k=130;gradT=htot/(k)*(Tinf-T);";
}

The results show different gradient values on the walls, gradTx, gradTy and gradTz are so much more that the input values. I should mention that when I apply this BC for top surface which is horizontal I get perfect results. Here it says ( http://www.foamcfd.org/Nabla/guides/...Guidese11.html) that by "fixedgradient" we define
. I need to define only the magnitude of temperature gradient on the tubes.

Could you help me please?

Thank you

aa

[matthi]

Hello Socrates,

I don`t understand your physical problem and why you need a fixed gradient. May be you could also use a fixed heat flux?
Nevertheless, I have some experience in defining boundary conditions for solid regions. Maybe, you find something useful in the solver:

OpenFOAM-1.7.\applications\solvers\heatTransfer\chtMultiReg ionSimpleFoam

The boundary conditions can be find in the subfolder

derivedFvPatchFields\solidWallHeatFluxTemperature

Good luck

Matthi

[jorkolino]

Originally Posted by mabinty

That means you did not specify how the conductivity fied "K" shoud be calculated. Look at the top of src/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.H:

hotWall
        {
            type            compressible::turbulentHeatFluxTemperature;
            heatSource      flux;        // power [W]; flux [W/m2]
            q               uniform 10;  // heat power or flux
            K               basicThermo; // calculate K by alphaEff*thermo.Cp
            value           uniform 300; // initial temperature value
        }

Cheers,
Aram

In my case, the error message says keyword alphaEff is undefined. Shall I use the same assignment as for the K keyword above? Forgot to mention, my solver buoyantBoussinesqSimpleFoam. Nope, it does not work, I tried define the alphaEff keyword as above, but it is rejected as a valid entry in the basicThermo.

[rahulps]

--> FOAM FATAL IO ERROR:
keyword kappa is undefined in dictionary "/home/rahulps/OpenFOAM/rahulps-2.2.2/run/conjugate1/0/solid/T.boundaryField.solid_to_fluid"

file: /home/rahulps/OpenFOAM/rahulps-2.2.2/run/conjugate1/0/solid/T.boundaryField.solid_to_fluid from line 41 to line 45.

From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 402.

FOAM exitin

[Naresh yathuru]

Hi Foamers,

I m using openFoam 2.3.0 and the solver is buoyantBoussinesqsimpleFoam. I am simulating a room with a cube inside i have to impose heat flux boundary conditions..Therefore i applied turbulentHeatFluxTemperature bc for the patch as follows
innercube
{
type turbulentHeatFluxTemperature;
heatSource flux; //power;
q uniform 100;
value uniform 293.0;
}

Now i m getting a error as innercube

keyword alphaEff is undefined in dictionary "/home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube"
[7]
[7] file: /home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube from line 40 to line 43.
[7]
[7] From function dictionary::lookupEntry(const word&, bool, bool) const
[7] in file db/dictionary/dictionary.C at line 437.
[7]
FOAM parallel run exiting

I have read in the forum that i should change kappaeff to alphaeff in th Tequ.H but it turns out the new version already has the changes implimented. so i m not sure where i m went wrong.
could someone please help help me. im desperate for help.

[Naresh yathuru]

Hi rahul and george

i have a similar error how did u alble to solve your error coul you please help me.

Thankyou

regards,
Naresh

[agustinvo]

Originally Posted by Naresh yathuru

Hi Foamers,

I m using openFoam 2.3.0 and the solver is buoyantBoussinesqsimpleFoam. I am simulating a room with a cube inside i have to impose heat flux boundary conditions..Therefore i applied turbulentHeatFluxTemperature bc for the patch as follows
innercube
{
type turbulentHeatFluxTemperature;
heatSource flux; //power;
q uniform 100;
alphaEff alphaEff;
value uniform 293.0;
}

Now i m getting a error as innercube

keyword alphaEff is undefined in dictionary "/home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube"
[7]
[7] file: /home/yathuru/praktikum/noniso/heat_transfer_flux/processor7/0/T.boundaryField.innercube from line 40 to line 43.
[7]
[7] From function dictionary::lookupEntry(const word&, bool, bool) const
[7] in file db/dictionary/dictionary.C at line 437.
[7]
FOAM parallel run exiting

I have read in the forum that i should change kappaeff to alphaeff in th Tequ.H but it turns out the new version already has the changes implimented. so i m not sure where i m went wrong.
could someone please help help me. im desperate for help.

Hello

You have to declare inside your BC which variable would be your alphaEff. Otherwise the BC code cannot continue.

In relation with the name of the variable, it does not matter if you have defined it in the solver. So you could put

alphaEff alphaEff;

or

alphaEff kappaEff;

[Naresh yathuru]

Hi augstin villa and other Foamers,

Thanks for your reply.

It took me a some time to find it out and itseems nobody left any trace of the changes in new version but i m glad to share this. In openFoam version 2.3.0 the thermal diffusivity kappaeff in turbulence heatflux temperature is already replacded to alphaeff.

And aditionally u have to include Cp0 Cp0 1005 in the ttransport properties. Note (no dimention for Cp0)

Fore more details check turbulenceheatfluxtemperature.H

hope this would help people like me who arre new to openFoam

Regards,
Naresh

[dewey]

Hi

Do you know how i can use the heat flux as Bc on a wall with a buoyantBoussinesqSimpleFoam, something like INcompressible::turbulentHeatFluxTemperature??

[dewey]

i found this

https://github.com/OpenFOAM/OpenFOAM...hScalarField.H

But when i search in my OF 4.1 i cant find it, and i dont know how to add it.

[agustinvo]

Originally Posted by dewey

i found this

https://github.com/OpenFOAM/OpenFOAM...hScalarField.H

But when i search in my OF 4.1 i cant find it, and i dont know how to add it.

Hello dewey,

last week I have been working in the code to use the compressible::turbulentHeatFluxTemperature in a incompressible solver. I can share with you the code, but it would be tomorrow.

[jeanpinto24|]

I have a doubt. In my case I have to add the heat contributed by the people in my simulation. The question that comes to me when using the BC: turbulentHeatFluxTemperature will I see in my simulation the outflow of heat from the wall?

[ketanganatra0@yahoo.com]

it is the mode that you have to define either flux or power
type compressible::turbulentHeatFluxTemperature;
heatSource flux; // power [W]; flux [W/m2]
q uniform 10; // heat power or flux
kappa fluidThermo; // calculate kappa=alphaEff*thermo.Cp
Qr none; // name of the radiative flux
value uniform 300; // initial temperature value

[calf.Z]

Originally Posted by mabinty

Hi,

value             uniform 293.0;

is used as initial value at the respective patch. To check wall heat fluxes use the "wallHeatFlux" utility.

Aram

If I use wallHeatFlux to check the heat flux. Should the value be the same as the setting one in externalWallHeatFluxTemperature BC ? If the two values are different, what is the reason of it? Thank you.