CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

cp field in buoyantBoussinesqSimpleFoam for turbulentHeatFluxTemperature

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   January 20, 2011, 05:43
Default cp field in buoyantBoussinesqSimpleFoam for turbulentHeatFluxTemperature
  #1
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: Stockholm, Sweden
Posts: 359
Rep Power: 11
romant is on a distinguished road
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
    }
__________________
~roman
romant is offline   Reply With Quote

Old   January 20, 2011, 06:18
Default
  #2
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
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
fcollonv is offline   Reply With Quote

Old   January 21, 2011, 07:31
Default
  #3
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 237
Rep Power: 9
olivierG is on a distinguished road
hello,
A more easy way should be to set Cp to the correct value, like
Code:
Cp 1000;
for air.

Regards,
olivier
olivierG is offline   Reply With Quote

Old   December 23, 2012, 18:52
Default
  #4
New Member
 
Luke
Join Date: Jul 2012
Posts: 2
Rep Power: 0
MrFrog is on a distinguished road
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
MrFrog is offline   Reply With Quote

Old   January 2, 2013, 04:55
Default
  #5
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 237
Rep Power: 9
olivierG is on a distinguished road
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
olivierG is offline   Reply With Quote

Old   January 30, 2013, 00:31
Default
  #6
New Member
 
Luke
Join Date: Jul 2012
Posts: 2
Rep Power: 0
MrFrog is on a distinguished road
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
MrFrog is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Phase Field modeling in OpenFOAM adona058 OpenFOAM Running, Solving & CFD 24 January 31, 2015 07:01
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Turbulence dampening due to magnetic field in LES and RAS eelcovv OpenFOAM 0 June 8, 2010 11:35
Zero size field taranov OpenFOAM Bugs 2 April 20, 2010 04:51
Problem with rhoSimpleFoam matteo_gautero OpenFOAM Running, Solving & CFD 0 February 28, 2008 07:51


All times are GMT -4. The time now is 07:17.