# Natural Convection, Urgent

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

 LinkBack Thread Tools Display Modes
 September 25, 2003, 12:50 Natural Convection, Urgent #1 elyyan Guest   Posts: n/a hi, this is the second message I post on the issue of natural convection, some of the guys gave me some good advices about the issue and what steps I should take, but it did not converge. my simulation again is a closed 3D single zone filled with gas and differentially heated, my Ra is 10^10 (which is obviously turbulent), I have tried to approach the application fllowing Fluent's manual by starting with Ra 10^7 and then increase it to 10^10, it did not work. I would like to know: 1. which trubulent model to use and should I activate full bouyance effects or not. 2. should I use boussinesque approximation or a temperature dependent function for the density, or just put the ideal gas assuption for the material, 3. what are the undeerrlaxation factors that I should use. thanks alot for your help elyyan

 September 29, 2003, 04:36 Re: Natural Convection, Urgent #2 Martin Guest   Posts: n/a hi, 1. which turbulence model have you tried? 2. you can use boussinesque, but donīt forget to set thermal expansion coeff. under materials... 3. you can use the standard factors. it should work!

 September 29, 2003, 11:12 Re: Natural Convection, Urgent #3 elyyan Guest   Posts: n/a I have used the k-epsilon RNG model, and chosed the full bouyancy option, 2. I am using a temperature dependent density for my application, 3. unfortunately the standard underrelaxation coefficient are not working well, I am trying to play with them, but the natural convection is sensitive for them. If you have any ideas, I would be glad to know them. Thanks Elyyan

 September 29, 2003, 11:55 Re: Natural Convection, Urgent #4 Martin Guest   Posts: n/a hi, i think it is a grid-problem... how fine is the grid at the walls? what wall function do you use ???

 September 29, 2003, 13:31 Re: Natural Convection, Urgent #5 elyyan Guest   Posts: n/a I am using a standard wall function, in regard to the grid, my zone is just a closed box, and the grid is all hexa, i have used boundary layer mesh near the walls, i do not know do i need to make the mesh finer, or increase the boundary layer near the wall, if you have a good mesh scheme, I would appreciate it if you can provide me with it. Thanks Elyyan

 September 29, 2003, 22:06 Re: Natural Convection, Urgent #6 Jin-Wook LEE Guest   Posts: n/a You shoud have enough grid near the heated(or cooled) wall. This is, I think, the most important for natural convection. Boundary layer thickness of the natural convection in the cavity is order of Ra^(-1/4). As you may know, This boundary layer is 'physical boundary layer', not 'GAMBIT boundary layer'. Let me have order analysis for the natural convection in the cavity with differentially heated vertical side walls. In this case, characteristic length is witdth between two heated walls(one is, in general, cooling wall), say it as W. Your Ra is 10^10. So your boundary layer thickness is order of 10^(-2.5). That means, boundary layer thickness of the cavity is about 0.003W. In this narrow region, velocity changes very steeply. And the other region is, so called (nearly inviscid) core region. I think that AT LEAST 3 or 4 grid should be located in this narrow region. Then, grid size near the heated(or cooled) wall should be about 0.001W or smaller. For, your reference, I have met many CFD analysists who are complaining the divergence or unreasonable results for natural convection, who had coarse grid near the wall. 'ALL' of them were successfule for the simulation by fine grid near the wall. I hope that your case is also belong to this category. Sincerely, Jinwook

 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 NSV FLUENT 10 May 6, 2014 04:25 jorien CFX 0 October 14, 2011 09:26 Alex Siemens 5 December 12, 2007 05:58 alanna FLUENT 3 March 2, 2005 12:46 mauricio FLUENT 2 February 23, 2005 20:43

All times are GMT -4. The time now is 11:29.

 Contact Us - CFD Online - Privacy Statement - Top