CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Turbulent thermal conductivity (http://www.cfd-online.com/Forums/openfoam-solving/60222-turbulent-thermal-conductivity.html)

 newbee May 9, 2006 07:16

Hello, Im creating a case w

Hello,

Im creating a case whera a fluid of incompressible fluid is beeing heated from a constant heat flux from one of the walls.

As temperature B.C for that wall I have put upp the condition fixed gradien (uniform) which works fine. Th problem is which value to use for the konstant temperature gradient. Im using the formula deltaT=q''/kEff. The problem is to find a value for the constant kEff=kTurb+k (where kTurb is the problem) Deos anyone know how I can find this value out?

Thanks
/Erik

 Anne Lincke November 25, 2011 04:47

As far as I know k_eff = v/Pr + nu_t/Prt

where nu is the kinematic viscosity, nu_t the turbulent viscosity and Pr and Pr_t Prandtl-number, laminar and turbulent, respectively.

 Tiffany August 29, 2012 18:47

Hi Anne and Erik,

I'm new to OpenFOAM and CFD. I'm trying to determine the heat transfer from a problem I setup. It is a heated concentric cylinder problem that I solved with the k-epsilon model with buoyantBoussinesqPimpleFoam. It appears to solve for kappat (kinematic turbulent thermal conductivity), k (turbulent kinetic energy), nut (turbulent viscosity), alphat (thermal diffusivity), epsilon (kinetic energy dissipation rate), and a few others. I'm a little lost as to what equation to use to get the effective thermal conductivity though. If I can get k_eff, I have a formula for my particular setup to get the heat transfer. But I'm stuck on how to get k_eff. Any suggestions?

 Anne Lincke September 10, 2012 06:05

Hey Tiffany,

kappa_eff is the sum of kappa_t and kappa.
The ladder is computed from nu/Pr which are defined in constant/transportProperties.

Kind Regards
Anne

 palmerlee December 29, 2013 09:25

Hi, Tiffany!
Have you solve your problem yet? I have a similar question. As mentioned by Anne, k_eff = v/Pr + nu_t/Prt, then I guess k_eff is not a constant because nu_t is not. Am I right? If it is so, then how to set up the temperature boundary condition for a give heat flux?

Regards
Peter

 Anne Lincke January 8, 2014 09:08

Hey Peter,

there are wall functions for kappat, namely

Quote:
 kappatJayatillekeWallFunction
which you can use at the wall.

On the other boundaries you can set kappat to "calculated" as it is computed from nut, which is computed from the turbulent properties (omega, k, epsilon,...). You can also use "symmetryPlane" or "empty", depending on the case that you would like to simulate.

Kind Regards
Anne

 palmerlee January 8, 2014 21:10

Quote:
 Originally Posted by palmerlee (Post 468014) Hi, Tiffany! Have you solve your problem yet? I have a similar question. As mentioned by Anne, k_eff = v/Pr + nu_t/Prt, then I guess k_eff is not a constant because nu_t is not. Am I right? If it is so, then how to set up the temperature boundary condition for a give heat flux? Regards Peter
The following code is for those who need to set a fixed heat flux boundary:

Quote:
 wall { type groovyBC; value uniform 300; valueExpression "300"; gradientExpression "gradT"; fractionExpression "0"; variables ( "heatFlux=100;" "rho=1.1767;" "cp=1006.6;" "nv=1.58e-05;" "pr=0.714;" "kappa=nv/pr;" "gradT=heatFlux/((kappa+kappat)*rho*cp);" ); }

 palmerlee January 12, 2014 21:07

Hi, Anne!

Thank you for reply. Here is my kappt boundary:
Quote:
 wall { type fixedValue; value uniform 0; } top { type calculated; value \$internalField; } inlet { type calculated; value \$internalField; } outlet { type calculated; value \$internalField; }
The yPlus in my case is small (y+ < 3) so that I do not use wall funtion. Instead, I set it to zero at the wall. Please correct me if I am wrong. I use LES turbulent model.
By the way, my simulation seems to blow up after thousands of time steps and I have no idea what causes that. Could it be the fvSchemes?

Regards
Peter

 Anne Lincke January 13, 2014 04:32

Dear Peter,

I think if your mesh is fine enough you can set kappat like that.
What kind of boundary is boundary "Top" in your case?

In which sense does the simulation blow up? Residuals? Continuity error?

 palmerlee January 13, 2014 06:46

Dear Anne,

"Top" is an open boundary which I treated the same way as the "outlet" boundary. This is U at "top" boundary:
Quote:
 { type inletOutlet; inletValue uniform (0 0 0); value uniform (0 0 0); }
I set "adjustTimeStep" on to keep Co<0.5. For the first thousands of time steps, delta t is at the order of e-6 second, as it supposed to be. After that, delta t become extremely small. The latest time step is 2.46198e-18 second, for instance. Then I checked the velocity field and found it a total mess. The field became nonphysical.

Perhaps I should use the QUICK scheme for the discretization of the energy equation, the same way as a simulation work in literature.

Best,
Peter

 All times are GMT -4. The time now is 20:33.