CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Problem with Turbulent Heat Flux Temperature boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 7, 2014, 10:32
Default Problem with Turbulent Heat Flux Temperature boundary condition
  #1
New Member
 
Manuel
Join Date: Jan 2013
Posts: 21
Rep Power: 5
Manuel CFD is on a distinguished road
Dear All,

I have a problem with the compressible::turbulentHeatFluxTemperature boundary condition. I am performing an heat transfer computation with some heat source surfaces. On these surfaces I want to impose fixed heat fluxes (in the range 500-30000 W/m2). The problem I encounter is that, starting from the first iteration, the temperature diverges approaching unphysical values on the corresponding surfaces. I tried to bound the temperature (bounding value 2000 K). Unfortunately this does not help the temperature to approach realistic values and furthermore, using the wallHeatFlux utility I checked that the "real" heat fluxes acting on these surfaces are different from the imposed ones.
Have you got any idea about the reason why this problem happens??

Thank you.

Manuel
Manuel CFD is offline   Reply With Quote

Old   March 8, 2014, 17:01
Default
  #2
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 391
Rep Power: 11
jherb is on a distinguished road
What turbulent model are you using? What are the y+ values at the heated wall? Corresponding on the wall functions for kappa (or alpha) it is based on viscosity (mu_turbulent/Pr_turbulent). And for some wall functions of mu_turbulent, it might not be calculated if y+ is too small. So mu_turbulent might be only mu_laminar, so the heat transfer becomes much too low => temperature too high
jherb is offline   Reply With Quote

Old   March 10, 2014, 05:27
Default
  #3
New Member
 
Manuel
Join Date: Jan 2013
Posts: 21
Rep Power: 5
Manuel CFD is on a distinguished road
Dear jherb,

I am using the kEpsilon turbulence model, with wall functions only for k and epsilon (no wall functions for mut and alphat, they are simply calculated on the walls). I am using the wall functions even if the mesh is coarse at walls and yPlus is outside the log-law region. I can't avoid to have large yPlus values since my mesh is already very large and making it finer is not feaseable for me.
Should I use another treatment for turbulent quantities at walls? I tried to bypass the wall functions using directly fixed boundary conditions for k and epsilon (k, epsilon = 0 at walls). Anyway the solver automatically assigns the wall functions and does not consider my fixed value boundary conditions.
Have you any suggestions??

Thank you,

Manuel
Manuel CFD is offline   Reply With Quote

Old   March 10, 2014, 10:01
Default
  #4
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: London, UK
Posts: 368
Rep Power: 13
romant is on a distinguished road
Hej,

you need to set wall functions for alphat and mut as well. For mut you probably want to set mutkWallFunction and for alphat you can either use alphatWallFunction, which is very basic or alphatJayatillekeWallFunction, which is a more advanced wall function which gives good values over a large range of Reynolds and Prandtl numbers.
__________________
~roman
romant is offline   Reply With Quote

Old   March 10, 2014, 10:12
Default
  #5
New Member
 
Manuel
Join Date: Jan 2013
Posts: 21
Rep Power: 5
Manuel CFD is on a distinguished road
Dear romant,

Ok. I am going to try in accordance with your suggestions. Anyway, don't you think that applying wall functions outside their region of validity (I mean log-law layer) could be improper and/or lead to erroneous results?

Thank you,

Manuel
Manuel CFD is offline   Reply With Quote

Old   March 10, 2014, 10:18
Default
  #6
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: London, UK
Posts: 368
Rep Power: 13
romant is on a distinguished road
Yes, outside the region it will lead to erroneous results. However, the validity region is quite large 30<y+<150 (sometimes even larger). So if your mesh does not fall within this region, one option is to adapt the mesh.

You won't be able to have anything else at the wall, there is just no models (to my knowledge) that would support larger y+ at the wall and going with something that is laminar is definitely wrong.
__________________
~roman
romant is offline   Reply With Quote

Old   March 10, 2014, 10:41
Default
  #7
New Member
 
Manuel
Join Date: Jan 2013
Posts: 21
Rep Power: 5
Manuel CFD is on a distinguished road
Dear romant,

Ok. I'll try with these 2 wall functions and I'll let you know back.
Thank you,

Manuel
Manuel CFD is offline   Reply With Quote

Old   March 12, 2014, 07:11
Default
  #8
New Member
 
Manuel
Join Date: Jan 2013
Posts: 21
Rep Power: 5
Manuel CFD is on a distinguished road
Dear romant,

I tried to switch the turbulence model from k-epsilon to realizableKE. The latter one automatically assigns the wall functions for mut and alphat.
Unfortunately this has not brought up any improvement.
What do you suggest to do??

Manuel
Manuel CFD is offline   Reply With Quote

Old   March 12, 2014, 10:06
Default
  #9
Senior Member
 
romant's Avatar
 
Roman Thiele
Join Date: Aug 2009
Location: London, UK
Posts: 368
Rep Power: 13
romant is on a distinguished road
Try to set up a smaller case, similar in physics to the one you have and see if you can get it to work.

Also, you need to have your y+ in the range of the wall functions, this is then the coarsest you can go at the wall, otherwise your results will most likely be incorrect.

At the moment I would stay with just k-epsilon.

Which wall function do you use for mut, k, epsilon, alphat? Which boundary conditions do you have for p_rgh, U and T?
__________________
~roman
romant is offline   Reply With Quote

Old   March 12, 2014, 11:31
Default
  #10
Senior Member
 
Joachim Herb
Join Date: Sep 2010
Posts: 391
Rep Power: 11
jherb is on a distinguished road
You still have to specify the wall functions for mut and alphat in the corresponding files (mut and alphat in the 0 directory).

Quote:
Originally Posted by Manuel CFD View Post
Dear romant,

I tried to switch the turbulence model from k-epsilon to realizableKE. The latter one automatically assigns the wall functions for mut and alphat.
Unfortunately this has not brought up any improvement.
What do you suggest to do??

Manuel
jherb is offline   Reply With Quote

Old   March 17, 2014, 05:47
Default
  #11
New Member
 
Manuel
Join Date: Jan 2013
Posts: 21
Rep Power: 5
Manuel CFD is on a distinguished road
Dear All,

I thank you for your suggestions.
I remeshed the domain in order to guarantee a yPlus being in the validity range. In this way results quality improved significantly. The maximum temperature value is decreased drastically but it still remains unphysical. I would try to switch the turbulence model form realizableKE to k-w SST. Do you think that this change could produce better results? Do you have other suggestions?

Thank you,

Manuel
Manuel CFD is offline   Reply With Quote

Old   March 17, 2016, 16:12
Default
  #12
Member
 
Cong
Join Date: Nov 2012
Posts: 79
Rep Power: 6
wc34071209 is on a distinguished road
I am faced with the same problem here.
wc34071209 is offline   Reply With Quote

Reply

Tags
boundary condition, buoyant flows, heat flux, heat transfer, temperature bc

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
convergenceof natural convection prob. in cfx cpkewat CFX 15 January 31, 2014 07:29
Low Mixing time Problem Mavier CFX 5 April 29, 2013 00:00
Constant Heat Flux Boundary Condition on Long Thin Pipe CGramlich SU2 3 April 22, 2013 08:25
(Heattransfer) Temperature boundary condition problem suitup OpenFOAM Bugs 15 October 14, 2010 22:18
No results for solid domain Gary Holland CFX 10 March 13, 2009 04:30


All times are GMT -4. The time now is 01:38.