Discussion Groups

## Simulation CFD

New Member
Posts: 1
Registered: ‎10-05-2012

# Need basic help for convective heat transfer problem

191 Views, 1 Replies
10-05-2012 12:42 PM

So I have an enclosure that has various electrical parts like a power supply, relay, and i/o module and each has its own heat dissipation rate. I want to know what the temperature of the air in the enclosure will become if it is sealed. Once I get that, I'm hoping to put some vents on the enclosure and see how much the temperature goes down due to natural convection. And if I get both to work, I want to then do it with forced convection to see how much more I can get the temperature down.

So far, I've set the initial conditions of everything to 50 degrees C since that is my ambient temperature. I then set a boundary condition for each part that has a heat dissipation and gave it the appropriate number. I also made a large external volume to represent the air in the room that the enclosure will be in and set its boundary condition to 50 degrees C so that it won't change. For simplicity, I also made all my parts A36 Steel and the external volume air.

I ran the solver doing incompressible flow and auto forced convection for heat transfer. I do get temperature results, the hottest part goes from 50 C to 94 C but I don't see any flow visualization. I set up a plane and added trace points but don't see any movement. Shouldn't the auto forced convection create flow in this system? I've also tried making vents in the enclosure, creating an internal volume, and setting a boundary condition for the vents giving them a volumetric flow rate in to the enclosure at one end and out of the enclosure at the other end. I still don't get any flow visualization. This make me believe that the temperature results I'm getting are solely based off conduction.

Anything you guys see that I'm doing wrong?

Please use plain text.
Product Support
Posts: 729
Registered: ‎08-25-2011

# Re: Need basic help for convective heat transfer problem

10-08-2012 03:20 AM in reply to: AKhamesi

HI,

There are a few things wrong here, yes.

Firstly, I would suggest you may want to run with natural convection externally to the box anyway, then you can simply clone the design, add some vents and get a proper comparison of how each behave.

It is important to understand that (unless they are volumetric thermal loads applied to solids) Boundary Conditions (BC's) can only be applied to the external surfaces of a domain. Initial Conditions will do nothing on a steady state run, which this is, they are just a point in time used for transient analyses. Do not set the air-volume to 50C either, this is not strictly true, as it will heat up near the unit.

Here you need to place the unit inside an air-box, this should be roughly 6-8x lt's length/width in each direction and probably at least 8x in height (you need to capture the plume of heat well). Look in the help for a 'lighting guide' this shows the setup entirely, inclusing the air-box dimensions.

If this is desk mounted, place the unit at the bottom of this box (air domain) and simply apply a P=0 and a film coeff of 5W/m2/K @ ambient +1C on the top of the air domain. Those and the heat loads will be the only BC's you need.

The air must be set to air_variable or you will only have conduction and no convection - all this is in the help.

Physics: Be sure to turn on both heat transfer and gravity in the correct direction

Probably best to run with a Mixing Length turbulence model also, until you have forced convection, then you will need to go back to the default.

Hope that helps,

Jon

Jon Wilde
Please use plain text.