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

Turbulent thermal conductivity

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

Like Tree2Likes
  • 1 Post By Anne Lincke
  • 1 Post By Anne Lincke

Reply
 
LinkBack Thread Tools Display Modes
Old   May 9, 2006, 07:16
Default Hello, Im creating a case w
  #1
newbee
Guest
 
Posts: n/a
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
  Reply With Quote

Old   November 25, 2011, 04:47
Default
  #2
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
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.
Goutam likes this.
Anne Lincke is offline   Reply With Quote

Old   August 29, 2012, 18:47
Default
  #3
New Member
 
Anonymous
Join Date: Aug 2012
Posts: 8
Rep Power: 5
Tiffany is on a distinguished road
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?
Tiffany is offline   Reply With Quote

Old   September 10, 2012, 06:05
Default
  #4
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
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
Anne Lincke is offline   Reply With Quote

Old   December 29, 2013, 09:25
Default
  #5
Member
 
Peter
Join Date: Nov 2011
Posts: 45
Rep Power: 5
palmerlee is on a distinguished road
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
palmerlee is offline   Reply With Quote

Old   January 8, 2014, 09:08
Default
  #6
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
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 likes this.
Anne Lincke is offline   Reply With Quote

Old   January 8, 2014, 21:10
Default
  #7
Member
 
Peter
Join Date: Nov 2011
Posts: 45
Rep Power: 5
palmerlee is on a distinguished road
Quote:
Originally Posted by palmerlee View Post
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 is offline   Reply With Quote

Old   January 12, 2014, 21:07
Default
  #8
Member
 
Peter
Join Date: Nov 2011
Posts: 45
Rep Power: 5
palmerlee is on a distinguished road
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
palmerlee is offline   Reply With Quote

Old   January 13, 2014, 04:32
Default
  #9
Senior Member
 
Anne Gerdes
Join Date: Aug 2010
Location: Hamburg
Posts: 152
Rep Power: 7
Anne Lincke is on a distinguished road
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?
Anne Lincke is offline   Reply With Quote

Old   January 13, 2014, 06:46
Default
  #10
Member
 
Peter
Join Date: Nov 2011
Posts: 45
Rep Power: 5
palmerlee is on a distinguished road
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.

Thanks again for your reply.

Best,
Peter
palmerlee 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
Effective Thermal Conductivity Merlin CFX 2 July 23, 2015 07:10
thermal conductivity Cirilo CD-adapco 3 April 23, 2012 12:08
Anisotropic thermal conductivity Helger Dooley CFX 2 September 1, 2005 08:52
walls- thermal conductivity ana Main CFD Forum 1 July 14, 2005 18:16
thermal conductivity Magnus Rohde Phoenics 2 May 22, 2003 07:36


All times are GMT -4. The time now is 17:05.