CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Axial fan or blower cooling a hot object with recirculation (http://www.cfd-online.com/Forums/cfx/99977-axial-fan-blower-cooling-hot-object-recirculation.html)

mariconeagles96 April 17, 2012 10:40

Axial fan or blower cooling a hot object with recirculation
 
Hi guys! Hope you could give me some help on this.

My simulation involves cooling an object which is directly near the fan. The geometry have bad airflow patterns wherein there is recirculation on the fan. I have two openings and specify it as "openings" for im not sure where the air will go in or out of my system enclosure. Fan is running at 18000 rpm and when using an axial fan, air direction should be from fan to heating element. If i use the blower fan (9000 rpm), air direction is from heating element to blower fan. Since i have recirculation my heating element (copper at 70w) temperature is just increasing and increasing. Althought my flow is converge, temperature is still computing. I already checked the heat transfer option on fluid-solid interface, have material conductivity but i was expecting that temperature will eventually steady out just like with our experimental test. Im using sst, fluid models are fun runner (rotating domain) and mainfluid (stationary) solid models are heating element and the enclosure. What seems to be the error in my modelling? Hope you could share some thoughts. Thanks! :)

ghorrocks April 17, 2012 19:04

You probably need to move the boundaries further away from the region of interest to eliminate the problem of boundaries you do not know how to define.

Also, as the temperature increases other effects become important. For instance radiation becomes big very rapidly as temperature increases and that will tend to allow the temeprature to stabilise, but at a high temeprature.

mariconeagles96 April 17, 2012 22:39

1 Attachment(s)
Thanks ghorrocks!

I already made my openings long enough for my flow to go in/out of my main fluid domain but still can make it work. For radiation, I neglected this option since im just concerned on forced convection. To better understand my problem, please see attached image.

ghorrocks April 18, 2012 07:09

You will probably get convergence eventually in your model. It is just that the thermal time scale is much longer than the flow time scale so it will take a while to get there. If your model is steady state you can accelerate this using a solid time scale factor. If transient you cannot accelerate it and just have to be patient.

By not including radiation the body will be hotter than reality. You cannot ignore radiation if you only want the convective losses. You can ignore radiation if it is not a significant source of heat transfer. If you ignore a significant heat transfer effect your equilibrium temperature will be rubbish.

mariconeagles96 April 18, 2012 08:41

thanks for the help...actually i did some modification now on my model and it seems that my openings are very small thus creating a backflow within the system. I've enlarged my openings and temperature seemed to be steady-out and now comparable to my experiment results. how to speed up the solid timescale? are there tutorials in cfx? sorry i havent gone all thru the tutorials.

we are ignoring radiation cooling since in forced convection, radiation just accounts for 5% (number may not be exact but its very little in actual application) in heat transfer. For natural convection, yes we account for that.

Anyway, thanks! I will keep all your suggestions in an open mind.


All times are GMT -4. The time now is 20:21.