[Rackaitis]

I am calculating steady 2D heat transfer problem. The case is simple. One solid aluminium part (~4x3 m size) generates heat (1200 W/m3). Air surrounds this part. My task is to do conservative calculations and by conservative I mean the worst heat exchange. That means only laminar flow around this aluminium part where radiation is not taken in account. Air and aluminium properties are taken from standard Fluent database.

I am not sure how to setup boundary conditions between aluminium part and air, so left all default values (on interface walls set Thermal conditions as Heat Flux with default (zero) values). Solution converges very slowly. Temperature profile looks logical. Air velocity vectors are of order 1e-10 and this is the biggest problem. I do not understand how air heated to 200°C do not flow under convective forces (the gravitation is turned on). Maybe I set up boundary conditions incorrectly. The solution space has pressure-inlet and pressure-outlet zones. Does anyone have an idea what I did wrong?

Bellow are link to problem case:
https://drive.google.com/open?id=0B-...lo3WXBRaG9mc2s

and calculated data:
https://drive.google.com/open?id=0B-...DJQdjkzOFdteEE


I searched this forum a little bit and found one answer to simillar problem:

============
[swtbkim - August 7, 2014, 04:13]
Are you going with steady solver?
You should use unsteady solver when handling heat transfer problem
============

I want to calculate steady solution and I do not see reason why I should use unsteady solver.

Can anyone explane to me why velocities are so small?

[KaLium]

Unfortunately I can't load your data. Can you show some pictures?

[Rackaitis]

Thanks KaLium for interest.

I put all latest files (including images) on google drive:
https://drive.google.com/drive/folde...0k?usp=sharing


Bellow are images
Attaching temperature and velocity magnitude images from calculations and mesh on boundary.

Temperature


Velocity


Mesh on boundary

[LuckyTran]

Originally Posted by Rackaitis

============
[swtbkim - August 7, 2014, 04:13]
Are you going with steady solver?
You should use unsteady solver when handling heat transfer problem
============

I want to calculate steady solution and I do not see reason why I should use unsteady solver.

Can anyone explane to me why velocities are so small?

I don't see any reason yet why you need to do unsteady.

I'm too lazy to download your case and open it.

Are you using ideal gas law or Boussinesq approximation? What's your density?

The temperature profile does not look right at all. It looks like you have pure conduction and no flow.

[Rackaitis]

LuckyTran, you are right!
The temperature profile looks like in a conduction problem and no flow is observed. This is my biggest headache.
Please note, the geometry size is about 10 m wide and that explains no flow problem in most of the domain. Anyway, the mesh size near active element is 5 mm wide. I do expect some flow in this region. Unfortunately calculations do not show this.

Right now I am rethinking my problem. Most probably I missed something essential, something that led me to ill-composed problem.

[LuckyTran]

Are you using ideal gas law or Boussinesq approximation? What's your density?

[Rackaitis]

Thanks LuckyTran!

I used standard air with a constant Density. You made me to check this parameter. Now I changed it to incompressible-ideal-gas and finally I got a flow!

Thanks!