CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Solving natural convection

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   July 18, 2012, 22:08
Question Solving natural convection
  #1
New Member
 
Join Date: Jun 2012
Location: Melbourne
Posts: 14
Rep Power: 5
Shljuki is on a distinguished road
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.
Shljuki is offline   Reply With Quote

Old   July 19, 2012, 06:06
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
Shljuki likes this.
ghorrocks is offline   Reply With Quote

Old   July 19, 2012, 08:54
Default
  #3
New Member
 
Join Date: Jun 2012
Location: Melbourne
Posts: 14
Rep Power: 5
Shljuki is on a distinguished road
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?
Shljuki is offline   Reply With Quote

Old   July 19, 2012, 16:43
Default
  #4
Ayk
New Member
 
Aykut
Join Date: Jul 2012
Posts: 3
Rep Power: 5
Ayk is on a distinguished road
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
Ayk is offline   Reply With Quote

Old   July 19, 2012, 21:59
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 20, 2012, 01:01
Default
  #6
New Member
 
Join Date: Jun 2012
Location: Melbourne
Posts: 14
Rep Power: 5
Shljuki is on a distinguished road
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?
Shljuki is offline   Reply With Quote

Old   July 20, 2012, 01:06
Default
  #7
New Member
 
Join Date: Jun 2012
Location: Melbourne
Posts: 14
Rep Power: 5
Shljuki is on a distinguished road
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?
Shljuki is offline   Reply With Quote

Old   July 20, 2012, 14:27
Default
  #8
Member
 
Felggv's Avatar
 
Felipe Gobbi
Join Date: Apr 2012
Location: Brazil
Posts: 76
Rep Power: 5
Felggv is on a distinguished road
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
Felggv is offline   Reply With Quote

Old   July 20, 2012, 18:10
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   July 21, 2012, 11:27
Default
  #10
Member
 
Felggv's Avatar
 
Felipe Gobbi
Join Date: Apr 2012
Location: Brazil
Posts: 76
Rep Power: 5
Felggv is on a distinguished road
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!
Felggv is offline   Reply With Quote

Old   July 21, 2012, 12:57
Default
  #11
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
When talking about meshes, "fine" is usually used as the oppsite of "coarse".
flotus1 is offline   Reply With Quote

Old   July 21, 2012, 13:52
Default
  #12
Member
 
Felggv's Avatar
 
Felipe Gobbi
Join Date: Apr 2012
Location: Brazil
Posts: 76
Rep Power: 5
Felggv is on a distinguished road
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.
Felggv is offline   Reply With Quote

Old   July 22, 2012, 08:22
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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".
ghorrocks is offline   Reply With Quote

Old   July 30, 2012, 20:27
Default
  #14
New Member
 
Join Date: Jun 2012
Location: Melbourne
Posts: 14
Rep Power: 5
Shljuki is on a distinguished road
t vs st.jpg

Wall heat flux [W] on the surface with the highest Rayliegh number: transient versus steady state results - 460 seconds.
Shljuki is offline   Reply With Quote

Old   July 30, 2012, 23:55
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Reply

Tags
natural convection, solving

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
Orifice Plate with a fully developed flow - Problems with convergence jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24
Differences between serial and parallel runs carsten OpenFOAM Bugs 11 September 12, 2008 11:16
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 19:07


All times are GMT -4. The time now is 09:31.