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

Modelling the wall heat transfer

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

Like Tree2Likes
  • 1 Post By ksrivast
  • 1 Post By MFGT

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 2, 2021, 00:11
Default Modelling the wall heat transfer
  #1
New Member
 
Guillaume Beardsell
Join Date: Aug 2012
Posts: 17
Rep Power: 10
magicbretzel is on a distinguished road
Hi,

I ran an IC engine simulation and compared the wall heat transfer from Converge with the one obtained using the Woschni correlation (in GT-Power). The heat transfer predicted by Converge is 5 times smaller than the one predicted with the Woschni correlation. Is it common? I am running at fairly standard operating conditions.

Along those lines, I have a few questions regarding how to model the wall heat transfer with RANS:

1a) In "Boundary" --> "Temperature boundary condition" --> "Heat model", one of the options is to put "Global". What does this imply? Does it mean that the model specified in "Turbulence modelling" --> "Turbulence model" --> "Wall heat transfer model" is the one that is used for that particular wall?

1b) Is it the same for the option "Global" in "Near wall treatment"?

2) In Chapter 8 of the manual, the different models for wall heat transfer are described. However, it remains unclear which model should be used for regular-sized engine?

3) For a given mesh size, my yplus varies from 1 to 100. What should I do to improve the heat transfer predictions? I am using the RNG k-epsilon turbulence model, the O'kourke and Amsden wall heat transfer model, and "Standard wall function" for "Near wall treatment".

Best regards,
Guillaume
magicbretzel is offline   Reply With Quote

Old   March 2, 2021, 17:07
Default
  #2
Senior Member
 
ksrivast's Avatar
 
Kislaya Srivastava
Join Date: Sep 2017
Location: Convergent Science, Northville MI
Posts: 110
Rep Power: 5
ksrivast is on a distinguished road
Hello Guillaume,

Are you comparing your heat transfer coefficients (HTC) results or heat flux results? HTC values are kind of arbitrary and depend on your definition. CONVERGE uses near wall temperatures to evaluate HTCs. Other codes/models can use bulk fluid temperatures. And so forth. This can cause a severe mismatch in HTC comparison. Also ensure that the same wall temperatures are being enabled for both. How do your pressure plots match with experimental data?

1. a. GLOBAL implies the model selected in turbulence.in will be used for that boundary.
1. b. Above is same of near-wall treatment.

2. Our recommendation for typical ICE cases is the O'Rourke and Amsden heat transfer model. It has worked well for us in the past. At the end of the day, these are different models, with their own assumptions, and the user is free to select between them to improve their results. As our manual notes, Angelberger has shown to consistently predict lower wall heat flux and Han and Reitz typically predicts higher heat transfer, out of our available models. So the rule of thumb is, if you feel your heat transfer is high, switch to Angelberger/GruMo. If you feel it is low, switch to Han and Reitz.

3. Ideally we would like to have y+ values in the range of 30-100 where Standard wall functions are valid and work well. For ICE cases, you'll typically see higher y+ values, esp during combustion. While the models are typically robust with slightly higher y+, you can bring down the y+ values to recommended range by employing y+ AMR or boundary embedding. For low y+ values, you can select scalable wall functions or enhanced near-wall treatment to improve results.

If there is a strong concern about wall heat transfer results and switching between our available models don't improve your results, and you feel the Woschni correlation predicts the correct/better heat flux, you can consider incorporating this correlation into a heat transfer UDF.

Hope this helps,

Sincerely,
__________________
Kislaya Srivastava
Research Engineer | Applications
CONVERGECFD
ksrivast is offline   Reply With Quote

Old   March 2, 2021, 17:51
Default
  #3
New Member
 
Guillaume Beardsell
Join Date: Aug 2012
Posts: 17
Rep Power: 10
magicbretzel is on a distinguished road
Hi Kislaya,

Thank you for the prompt reply. I am comparing the heat flux (in Watts) by summing up the heat transfer values from the bound*-wall.out files. I will use the enhanced wall model as well as the y+ AMR embedding, and see if that impacts the results.
magicbretzel is offline   Reply With Quote

Old   March 2, 2021, 19:20
Default
  #4
New Member
 
Guillaume Beardsell
Join Date: Aug 2012
Posts: 17
Rep Power: 10
magicbretzel is on a distinguished road
Hi Kislaya, I switched to "Enhanced wall treatment" for "Near wall treatment". However, I am now getting this warning in converge.log for a significant portion of the timesteps:

turbulence iterations= 49 error_eps= 3.9816e-03 error_tke= 5.6267e-03 omega_eps= 7.0000e-01 omega_tke= 7.0000e-01
turbulence iterations= 50 error_eps= 3.7338e-03 error_tke= 5.2653e-03 omega_eps= 7.0000e-01 omega_tke= 7.0000e-01
max iterations exceeded on turbulence

recovering .... because transport equations did not converge or energy extrapolations


I don't get these recovery messages when I run with the "Standard wall function" option. What could I try to improve the situation?

I tried increasing the maximum number of iterations for the TKE and dissipation rate transport equations from 50 to 500, but I still reach the maximum number of iterations for a significant number of timesteps, because the residuals stop going down at some point in the iterating process.

Thank you,
Guillaume
magicbretzel is offline   Reply With Quote

Old   March 2, 2021, 19:29
Default
  #5
Senior Member
 
ksrivast's Avatar
 
Kislaya Srivastava
Join Date: Sep 2017
Location: Convergent Science, Northville MI
Posts: 110
Rep Power: 5
ksrivast is on a distinguished road
Hello Guillaume,

You could try the following :
1. Keep max_tke/eps iterations at 500 and lower the under-relaxation factors to 0.5 to see if it helps.
2. Consider lower cfl limits / time-steps. Recoveries indicate a desire by the solver for lower time-steps to be more stable and reach convergence criteria.
3. Wait for a while to see if the recoveries go away.

Let me know if you continue to face issues.

Sincerely,
magicbretzel likes this.
__________________
Kislaya Srivastava
Research Engineer | Applications
CONVERGECFD
ksrivast is offline   Reply With Quote

Old   March 3, 2021, 04:38
Default
  #6
Senior Member
 
Tobias
Join Date: May 2016
Location: Germany
Posts: 229
Rep Power: 8
MFGT is on a distinguished road
Quote:
Originally Posted by ksrivast View Post
2. Our recommendation for typical ICE cases is the O'Rourke and Amsden heat transfer model. It has worked well for us in the past. At the end of the day, these are different models, with their own assumptions, and the user is free to select between them to improve their results. As our manual notes, Angelberger has shown to consistently predict lower wall heat flux and Han and Reitz typically predicts higher heat transfer, out of our available models. So the rule of thumb is, if you feel your heat transfer is high, switch to Angelberger/GruMo. If you feel it is low, switch to Han and Reitz.
I made an investigation of all 4 heat transfer models recently and found GruMo-UniMORE to be very similar to O'Rourke and Amsden heat transfer model, with a reduction by ~10%.

Starting with O'Rourke and Amsden, Angelberger had ~40% less Heat Transfer, while Han & Reitz had ~50% more Heat Transfer (calculated in kW).


Investigated engine was a 1.5L DI 4 cylinder at rated Power.
magicbretzel likes this.
MFGT is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Natural convection in a closed domain STILL NEEDING help! Yr0gErG FLUENT 4 December 2, 2019 00:04
surface heat transfer coeff of wall flux rsa FLUENT 0 June 1, 2016 09:40
Use of Wall Function Heat Transfer co-efficient mohibanwar FLUENT 1 September 8, 2015 01:02
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 06:20
Convective / Conductive Heat Transfer in Hypersonic flows enigma Main CFD Forum 2 November 1, 2009 22:53


All times are GMT -4. The time now is 00:50.