CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   heat transfer with laminar flow (http://www.cfd-online.com/Forums/openfoam/72316-heat-transfer-laminar-flow.html)

David_010 February 2, 2010 08:01

heat transfer with laminar flow
 
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.

Thomas Baumann February 2, 2010 11:32

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

David_010 February 2, 2010 11:52

Thankyou very much Thomas, I will try with the two options.

Regards

panda60 February 3, 2010 01:34

Quote:

Originally Posted by Thomas Baumann (Post 244621)
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.
http://www.cfd-online.com/Forums/ope...planation.html

David_010 February 3, 2010 08:01

Pressure conditions
 
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

panda60 February 3, 2010 10:02

Quote:

Originally Posted by David_010 (Post 244757)
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.

David_010 February 4, 2010 04:06

Yes Im simulating laminar flow, I use those boundary conditions just for laminar flow. Sorry

David

Thomas Baumann February 4, 2010 05:56

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

panda60 February 4, 2010 20:48

Quote:

Originally Posted by Thomas Baumann (Post 244900)
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 ?
http://www.cfd-online.com/Forums/ope...anation-2.html

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 ?

Thomas Baumann February 5, 2010 04:08

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

DineshramBalaji November 16, 2012 17:05

Adding temperature to icoFoam
 
Quote:

Originally Posted by Thomas Baumann (Post 244621)
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?


All times are GMT -4. The time now is 12:16.