# Solving natural convection

 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 18, 2012, 22:08 Solving natural convection #1 New Member   Join Date: Jun 2012 Location: Melbourne Posts: 14 Rep Power: 7 Sponsored Links Hi, i have a box model (room) with one cooled surface (ceiling) and one heated surface (window) and i am trying to solve the temperature field inside the room. There is no forced air flow and generated air movement is only due to natural convection, buoyancy effetc. I have a fine mesh, starting with 3mm cell height along the walls and inflation factor of 1.2. I am using k-w with automatic wall treatment. It is a stady state run. The solution reaches convergancy of about 5E-04. At this stage i stop solving fluids and turbulance and continue to solve only energy and radiation till the temperature field stabilise. Can you please advise if this methodology seems reasonable? Alse please advise on any other solving approach.

July 19, 2012, 06:06
#2
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,732
Rep Power: 106
Quote:
 I have a fine mesh
Do you know how many times I have heard that on the forum

Unless you have done a mesh sensitivity study and proved you have a fine mesh then you have an unknown mesh.

Quote:
 It is a stady state run.
Buoyant flows at Rayleigh numbers high enough to generate turbulence are almost always transient.

Quote:
 The solution reaches convergancy of about 5E-04. At this stage i stop solving fluids and turbulance and continue to solve only energy and radiation till the temperature field stabilise. Can you please advise if this methodology seems reasonable? Alse please advise on any other solving approach.
Have a look at this FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Reasonable - answer = no. You will have a big error.
Other approach - answer = transient solutions are almost always required for these sort of flows.

 July 19, 2012, 08:54 #3 New Member   Join Date: Jun 2012 Location: Melbourne Posts: 14 Rep Power: 7 Thanks for your reply. The meshing approach, first cell size and inflation has been documented as a reasonable good approach for natural convection studies. I have done a sensitivity check on a 2D simplified model against a mesh with Y+ of 0.9. Mesh seems fine. I have started with transient runs as transient behaviour of flow was expected. The transient runs take too long and they are dependant on initial guess. Since I had 20+ runs and not much time I looked for another solving approach and thought that running only energy and radiation at the end might provide a reasonable solution for comparative studies between the cases. The most relevant parameter for my study is the heat flux (cooling power or energy) supplied from ceiling surface into the domain and controlled by sensed temperature at the point. I have run one case in transient mode using converged steady state as initial condition and got difference of less than 3% for heat flux, which is acceptable for my analysis. Is this a typical error or I was just lucky with this one. We have one company licence and unfortunately I won't be able to test each case so I need a help with this issue. Is there any document or paper that addresses or quantifies this type of error to the solving approach I used in my analysis?

 July 19, 2012, 16:43 #4 New Member   Aykut Join Date: Jul 2012 Posts: 3 Rep Power: 7 Is not the SST Model recommended . k-w is well for the near wall regions but the more you get away from the wall it will lose accuracy as far as i know. There is also a max timestep you can set on buoyancy driven flows in the user manuals. That could help too for better convergence. And are your global imbalances ok ? Last edited by Ayk; July 19, 2012 at 16:44. Reason: forgot something

 July 19, 2012, 21:59 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,732 Rep Power: 106 The FAQ I linked to describes the process to go through. But if at the end of the day it means a transient run is required then anything else will cause significant error.

 July 20, 2012, 01:01 #6 New Member   Join Date: Jun 2012 Location: Melbourne Posts: 14 Rep Power: 7 Thanks Ayk, global imbalances are OK. The highest imbalance of for energy, still less than 1%. What turbulence model is recommended for natural convection analysis?

 July 20, 2012, 01:06 #7 New Member   Join Date: Jun 2012 Location: Melbourne Posts: 14 Rep Power: 7 Thanks Glenn, Rayleigh number in the worst case scenario is 6.88*10^8. I assume this indicates transition from laminar to turbulence flow. I will run the case with highest Rayliegh number in transient mode. Is there a way to plot Rayliegh number in CFX post, or it needs to be calculated?

 July 20, 2012, 14:27 #8 Member     Felipe Gobbi Join Date: Apr 2012 Location: Brazil Posts: 76 Rep Power: 7 Hello, I hope you don't bother if I come up with a discussion about mesh here in your topic since you said you had a "fine mesh". A friend of mine have generated a mesh on ICEM that had been through the quality test of ICEM and got min average 0.99 and max average 1.0. Should it be called a fine mesh? It's a Hexadominant mesh done manually by blocking method with 4.0cm sizing HVAC simulation with people represented by rectangular blocks with heat transfer. Thanks

 July 20, 2012, 18:10 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,732 Rep Power: 106 Rayliegh number is a global non-dimensional number, so you will need to calculate it. Sounds like the simulation is at least partly turbulent based on that Ra number. Felipe - mesh "fineness" has nothing to do with quality. They are independant parameters.

 July 21, 2012, 11:27 #10 Member     Felipe Gobbi Join Date: Apr 2012 Location: Brazil Posts: 76 Rep Power: 7 You mean fine in the sense of small elements? I misunderstood the meaning of his phrase: "I have a fine mesh". I thought fine meant good quality. By the way, if fine doesn't mean small elements, would you explain me or show an explanation of what does it mean? Thanks!

 July 21, 2012, 12:57 #11 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,506 Rep Power: 25 When talking about meshes, "fine" is usually used as the oppsite of "coarse".

 July 21, 2012, 13:52 #12 Member     Felipe Gobbi Join Date: Apr 2012 Location: Brazil Posts: 76 Rep Power: 7 When I read ghorrock's comment about the author of the topic saying he had a fine mesh and about sensitivity analysis and etc made me think that fine was about the quality since fineness is usualy "easy" to see since most computers here where I work cannot run simulations with meshes that are excessively fine.

 July 22, 2012, 08:22 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,732 Rep Power: 106 Yes, I can see now the word "fine" is ambiguous. I can see how people read it differently. My comment was assuming the small size definition of "fine".

 July 30, 2012, 20:27 #14 New Member   Join Date: Jun 2012 Location: Melbourne Posts: 14 Rep Power: 7 t vs st.jpg Wall heat flux [W] on the surface with the highest Rayliegh number: transient versus steady state results - 460 seconds.

 July 30, 2012, 23:55 #15 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,732 Rep Power: 106 Looks like you are getting transient behaviour, but the difference from the steady state run is small. So you will have to decide whether the extra effort of a transient solution is worth the extra accuracy.

 Tags natural convection, solving

 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 Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20 jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24 carsten OpenFOAM Bugs 11 September 12, 2008 11:16 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58 liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07