CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   cp field in buoyantBoussinesqSimpleFoam for turbulentHeatFluxTemperature (http://www.cfd-online.com/Forums/openfoam-solving/84107-cp-field-buoyantboussinesqsimplefoam-turbulentheatfluxtemperature.html)

romant January 20, 2011 05:43

cp field in buoyantBoussinesqSimpleFoam for turbulentHeatFluxTemperature
 
Hej,

I would like to use the turbulentHeatFluxTemperature boundary condition for a case solved with buoyantBoussinesqSimpleFoam. From discussions here in the forum I have already found that the alphaEff field should be the kappaEff, therefore I set this already. Unfortunately, I haven't been able to figure out how to set cp for this boundary condition, since there is no field for this available, and even if I create a field "cp" in the 0 folder, I can't use this one.

my boundary condition is set up like this
Code:

    heatedWall
    {
        type            turbulentHeatFluxTemperature;
        q              uniform 860.658e3;
        alphaEff        kappaEff;
        Cp              cp; // here I don't know what to set
    }


fcollonv January 20, 2011 06:18

Hello Roman,

I don't know about that boundary condition but after having a look to the code here is the problem. In buoyantBoussinesqSimpleFoam, the flow is incompressible basically. So the thermo variable available are restraint to the viscosity. And you don't have any Cp field available.

One solution could be to add the Cp field. But it is not sufficient to add it in the 0 folder you will have also to add it to the solver in "createFields.H" (look how is done for the temperature field). So it will be then available for the boundary condition.

Or the EASY way (better?), use buoyantSimpleFoam. For with it everything will be simpler.

Regards,

Frederic

olivierG January 21, 2011 07:31

hello,
A more easy way should be to set Cp to the correct value, like
Code:

Cp 1000;
for air.

Regards,
olivier

MrFrog December 23, 2012 18:52

I'm new to openfoam and I have the same problem did anyone solve this without having to re-compile it? I suspect there is an easier fix as it seems so simple. In buoyantBoussinesqPisoFoam (and i guess in bBSimpleFOAM too) the boundary condition asks for a volScalarField value so setting:

Cp Cp 1000; // didn't work obviously

I suspect I misunderstood OliverG but anymore advice on this would be great!

Thanks

F

olivierG January 2, 2013 04:55

hello,

You don"t need to add a VolScalarField if your Cp is constant, just use turbulentHeatFluxTemperature like:
Code:

heatedWall
    {
        type            turbulentHeatFluxTemperature;
        heatSource      power;// or flux
        q              uniform 80;
        alphaEff        kappaEff;
        Cp              uniform 1000;// Cp value here
        value          uniform 300;
    }

regards,
olivier

MrFrog January 30, 2013 00:31

Hello oliver,

First, thankyou for replying. Unfortunately this did not solve my problem. I think its because I am useing the OpenFOAM-1.6-ext project. I am told it's better and has more features, I wouldn't mind knowing which version of OF are you running and why? The error I encountered simply says:

--> FOAM FATAL ERROR:

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

8
(
rhok
kappaEff
nut
k
nu
p
T
epsilon
)


the full error:

HTML Code:

Build  : 1.6-ext-959ec266ba5c
Exec  : buoyantBoussinesqPisoFoam
Date  : Jan 30 2013
Time  : 03:44:40
Host  : john-Dell-System-XPS-L702X
PID    : 3379
Case  : /home/joebloggs/Documents/test/HexHeatFlux_I_tHFTemp
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


Reading g
Reading thermophysical properties

Reading field T

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Creating turbulence model

Selecting turbulence model type RASModel
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
    Cmu            0.09;
    C1              1.44;
    C2              1.92;
    sigmaEps        1.3;
}

Courant Number mean: 0 max: 0 velocity magnitude: 0

Starting time loop

Time = 0.2

Courant Number mean: 0 max: 0 velocity magnitude: 0
DILUPBiCG:  Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 2.69687e-06, No Iterations 9


--> FOAM FATAL ERROR:

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

8
(
rhok
kappaEff
nut
k
nu
p
T
epsilon
)


    From function objectRegistry::lookupObject<Type>(const word&) const
    in file /home/john/OpenFOAM/OpenFOAM-1.6-ext/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 140.

FOAM aborting

Aborted (core dumped)

frog


All times are GMT -4. The time now is 04:00.