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

heat transfer with laminar flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 2, 2010, 08:01
Default heat transfer with laminar flow
  #1
Member
 
David
Join Date: Dec 2009
Location: Spain
Posts: 58
Rep Power: 7
David_010 is on a distinguished road
Hi

I want to simulate a heat transfer problem with laminar flow. It consists on a circular duct with constant heat flux in the wall. For solve the hydrodynamic problem I have used the solver icoFoam, but, what solver can I use for the thermal problem?

Thankyou very mach for your attention.
David_010 is offline   Reply With Quote

Old   February 2, 2010, 11:32
Default
  #2
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi David,

you can modify the icoFoam solver for heat transfer problems. There's a tutorial of the wiki:
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

But it' s easier to use a turbulent solver with heat transfer and set as turbulence model in the RASproperties: laminar (for example buoyantBoussinesqSimpleFoam).

Regards

Thomas
Thomas Baumann is offline   Reply With Quote

Old   February 2, 2010, 11:52
Default
  #3
Member
 
David
Join Date: Dec 2009
Location: Spain
Posts: 58
Rep Power: 7
David_010 is on a distinguished road
Thankyou very much Thomas, I will try with the two options.

Regards
David_010 is offline   Reply With Quote

Old   February 3, 2010, 01:34
Default
  #4
Senior Member
 
Jiang
Join Date: Oct 2009
Location: Japan
Posts: 186
Rep Power: 7
panda60 is on a distinguished road
Quote:
Originally Posted by Thomas Baumann View Post
Hi David,

you can modify the icoFoam solver for heat transfer problems. There's a tutorial of the wiki:
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

But it' s easier to use a turbulent solver with heat transfer and set as turbulence model in the RASproperties: laminar (for example buoyantBoussinesqSimpleFoam).

Regards

Thomas
Dear ,Thomas
What boundary condition should I use for pressure ?
my flow is from inlet to outlet,
I have try all kind of boundary condition for pressure, but all does'nt converge.
could you help me ?

Thank you very much.
buoyantBoussinesqPisoFoam: A detailed explanation
panda60 is offline   Reply With Quote

Old   February 3, 2010, 08:01
Default Pressure conditions
  #5
Member
 
David
Join Date: Dec 2009
Location: Spain
Posts: 58
Rep Power: 7
David_010 is on a distinguished road
Hi

I can tell you the boundary conditions for pressure I'm using. In the inlet pressure is zeroGradient condition and in the outlet is fixed to 0. For the velocity in the inlet I'm using a uniform value and in the inlet zeroGradient condition. The results are successful with these conditions.

I hope it help you

David
David_010 is offline   Reply With Quote

Old   February 3, 2010, 10:02
Default
  #6
Senior Member
 
Jiang
Join Date: Oct 2009
Location: Japan
Posts: 186
Rep Power: 7
panda60 is on a distinguished road
Quote:
Originally Posted by David_010 View Post
Hi

I can tell you the boundary conditions for pressure I'm using. In the inlet pressure is zeroGradient condition and in the outlet is fixed to 0. For the velocity in the inlet I'm using a uniform value and in the inlet zeroGradient condition. The results are successful with these conditions.

I hope it help you

David
Dear David,
Are you simulating laminar flow ? I use kEpsilon buoyantBoussinesqSimpleFoam solver for turbulent flow, these boundary condition is not good for buoyantBoussinesqSimpleFoam.
panda60 is offline   Reply With Quote

Old   February 4, 2010, 04:06
Default
  #7
Member
 
David
Join Date: Dec 2009
Location: Spain
Posts: 58
Rep Power: 7
David_010 is on a distinguished road
Yes Im simulating laminar flow, I use those boundary conditions just for laminar flow. Sorry

David
David_010 is offline   Reply With Quote

Old   February 4, 2010, 05:56
Default
  #8
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi all,

I'm using buoyantBoussinesqSimpleFoam with turbulence models.

I'm using for the inlet: u fixedValue, p zeroGradient, k fixedValue, Epsilon fixedValue, T fixedValue.

for the outlet: u,k,Epsilon,T zeroGradient and for p fixedValue.


I've solved easy simulations like a turbulent pipe flow...

The simulation is more stable, if you use a hydraulicly developed inlet values (mapped boundary conditions) for k, epsilon, U. You must be careful for your inletValues of k and epsilon (omega).

Regards Thomas
Thomas Baumann is offline   Reply With Quote

Old   February 4, 2010, 20:48
Default
  #9
Senior Member
 
Jiang
Join Date: Oct 2009
Location: Japan
Posts: 186
Rep Power: 7
panda60 is on a distinguished road
Quote:
Originally Posted by Thomas Baumann View Post
Hi all,

I'm using buoyantBoussinesqSimpleFoam with turbulence models.

I'm using for the inlet: u fixedValue, p zeroGradient, k fixedValue, Epsilon fixedValue, T fixedValue.

for the outlet: u,k,Epsilon,T zeroGradient and for p fixedValue.


I've solved easy simulations like a turbulent pipe flow...

The simulation is more stable, if you use a hydraulicly developed inlet values (mapped boundary conditions) for k, epsilon, U. You must be careful for your inletValues of k and epsilon (omega).

Regards Thomas
Hi, Thomas,
Could come here to have a look at my case ?
buoyantBoussinesqPisoFoam: A detailed explanation

I have been struggling for this for a long time. I alse use kEpsilon model. In the begining, I use the same boundary condition with you, but it does not converge at all. Then I try to all kinds of boundary conditions for p, but all does not converge.
buoyantPressure can be used for outlet ?
I use upwind scheme, is it right for buoyantBoussinesqSimpleFoam ?
panda60 is offline   Reply With Quote

Old   February 5, 2010, 04:08
Default
  #10
Member
 
Join Date: Apr 2009
Location: Karlsruhe, Germany
Posts: 96
Rep Power: 8
Thomas Baumann is on a distinguished road
Hi panda60,

if you use buoyantBoussinesqSimpleFoam you have be sure that you are allowed to use the boussinesq-approximation (density changes should be very small). If not you should maybe use a compressible solver and modify it that the ideal gas law is not taken, but some other density-changes-rules.

Have you simulated the testcase with simpleFoam and it converged?

Here is my modus operandi:
1) Simulate the testcase laminar (simpleFoam and turbulence-model to laminar), sometimes you have to set the viscosity to a higher value, that it converges, because you simulate a turbulent Reynolds-area, but with laminar flow.
2) Simulate the testcase turbulent, but isothermal (simpleFoam), to be sure that your bc's for k, epsilon or whatever are okay. Maybe you have to change some of the relaxation-parameters for better residuals (make them smaller if the resiudals are swinging).
3) Simulate the turbulent and heated flow-problem at the end. (buoyantBoussinesqSimpleFoam)

Here are some hints:
If you set the gravity to zero you have no buoyant-forces in your simulation and the velocity-field of buoyantBoussinesqSimpleFoam should look the same as the SimpleFoam velocity-field.

If you have very small temperature-changes over the hole testcase, your residuals for T will take a long time (make the relaxation parameter for T to a higer value, e.d. 0.9).

I use upwind shemes for my first-order discretication solutions, too. For verification I put them to higher orders. But because of fine meshes I had no big changes of e.d. the velocity-profiles. I have never used buoyantPressure for outlet.

Regards Thomas

Last edited by Thomas Baumann; February 5, 2010 at 15:05.
Thomas Baumann is offline   Reply With Quote

Old   November 16, 2012, 17:05
Default Adding temperature to icoFoam
  #11
Member
 
Dinesh Balaji
Join Date: Oct 2012
Posts: 43
Rep Power: 4
DineshramBalaji is on a distinguished road
Quote:
Originally Posted by Thomas Baumann View Post
Hi David,

you can modify the icoFoam solver for heat transfer problems. There's a tutorial of the wiki:
http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

But it' s easier to use a turbulent solver with heat transfer and set as turbulence model in the RASproperties: laminar (for example buoyantBoussinesqSimpleFoam).

Regards

Thomas
Hi Thomas,

I am very new to openFoam. I tried modifying icoFoam to solve for temperature as instructed in "http://openfoamwiki.net/index.php/How_to_add_temperature_to_icoFoam". The final solution has results for only U, P and phi. I modified the files just like in the instructions. Can you suggest what might have gone wrong?
DineshramBalaji is offline   Reply With Quote

Reply

Tags
heat tranfer laminar

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
flow and heat transfer of rarefied air Jon FLUENT 0 October 23, 2008 16:23
2d Heat transfer external flow Richard belcher CFX 1 August 4, 2008 21:42
Two-Phase Buoyant Flow Issue Miguel Baritto CFX 4 August 31, 2006 12:02
Water vapour condensation in CFX-5.7.1 hdj CFX 1 November 27, 2005 08:15
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 12:57.