# Apparently we don't understand definition of "h"?!

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 October 17, 2005, 18:37 Apparently we don't understand definition of "h"?! #1 Chris Bailey Guest   Posts: n/a Sponsored Links OK, this is embarrasing, but a couple of us now are convinced we don't understand what heat transfer coefficient "h" means for an impinging jet on a surface. We calculate the flux at the surface, and divide that by the difference between the incoming fluid temperature and the surface temperature. Isn't that "h"? But we are a scientist using Fluent and an engineer using FloWorks, and each time we solve essentially the same problem, and ask the programs to calculate "h", they give us a result different from flux over delta temp. It's different by the same ratio in both environments, and the ratio is a function of both the high and the low temperatures. The ratios can be numbers like 0.6 or 2 or 30. Doing this point by point across the surface gives exactly the same ratio in both Fluent and FloWorks to several decimal places everywhere. What in the world are we too stupid to get here??? What do we completely misunderstand???
 Sponsored Links

 October 17, 2005, 18:45 Re: Apparently we don't understand definition of " #2 Jonas Larsson Guest   Posts: n/a Fluent uses a reference temperature set in the reference panel as the "bulk" (ie fluid) temperature. Did you set this to the correct incoming fluid temperature?

 October 17, 2005, 22:52 Re: Apparently we don't understand definition of " #3 Dong Ye Guest   Posts: n/a The temperature and heat flux are changing on the surface. h is different from point to point. Is there a mean heat flux and a mean temperature? So a general convective coefficient?

 October 18, 2005, 08:33 Re: Apparently we don't understand definition of " #4 ZubenUbi Guest   Posts: n/a It could also come from your test case. The value of h is correctly defined for a flow aligned with the plate where you compute h. For impinging jet, you may find something odd since the deformation tensor of the flow look strange. I know this have been corrected in some publications, but I can not find them now. May be you can googled it. Hopes that may help,

 October 18, 2005, 11:38 Jonas nailed it #5 Chris Bailey Guest   Posts: n/a Jonas, This looks like it. In Fluent there's a temperature setting "which is used to compute entropy for incompressible flows", according to the docs. I don't see it mentioned in discussions of heat transfer coefficients. But its default setting of 288.16 K or 15.01 C (?!) fits with my most recent experiment through 8 decimal places! But can this be the explanation in FloWorks? It would have to be the same bizarre value. Is 15.01 C the International Standard for Convected Air, or what? I'll ask the FloWorks user to try this. Thanks! - Chris

 October 18, 2005, 13:30 Re: Jonas nailed it #6 Scott Shaw Guest   Posts: n/a I think (haven't got reference materials to hand) 15 degrees C is standard sea-level temperature for an ISA (international standard atmosphere) day.

 October 18, 2005, 13:37 15.01 is standard #7 Chris Bailey Guest   Posts: n/a Sort of. I found it, since posting. 15.01 C is a standard atmosphere. I think maybe this odd number reflects a change in the definition of the Celsius scale - 1983, maybe?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post hjasak OpenFOAM Native Meshers: blockMesh 5 August 24, 2012 07:22 ljsh OpenFOAM Installation 82 October 12, 2009 11:47 Mauro Augelli (Augelli) OpenFOAM Installation 101 July 21, 2008 06:42 gschaider OpenFOAM Installation 118 July 20, 2008 05:19 fw407 OpenFOAM Paraview & paraFoam 6 May 30, 2008 17:09

 Sponsored Links

All times are GMT -4. The time now is 09:26.

 Contact Us - CFD Online - Top