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

Weller test case for XiFoam: results discrepancy

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 7, 2011, 12:17
Default Weller test case for XiFoam: results discrepancy
  #1
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
Dear foamers,

I'm trying to do the simulation used by Weller et al. to validate XiFoam
[H.G. Weller et al., 1998, Application of a Flame-Wrinkling LES Combustion Model to a Turbulent Mixing Layer, Twenty-Seventh Symposium (International) on Combustion/The Combustion Institute].

For that first I took simply the tutorial case, refine a bit the mesh at the shear layer and boundary layers and update the U and k file to use the experimental profiles.
Then the flame was effectively wrinkled (see XiFoamInit.jpg VS WellerResults.jpg - on the last the top picture is from the experiment). But the temperature and the pressure were crazy. In XiFoamInitTemperature.jpg I use a threshold filter to select the cells with a temperature between 260K and 290K. That range is totally unphysical as the temperature should not go below 293K.
So I changed the numerical schemes (cf. attachment). And now the pressure and the temperature are great: p is roughly constant and the minimal temperature is 292.6 K However the instability of the flame is gone.

Any suggestions will be appreciate.
Thanks,

Frederic

Additional information about the simulation:
* max CFL = 0.5
* no gravitation
* the mesh is not has large in the homogeneous direction as in the Weller's paper. The dimensions are those of the tutorial case
* the combustion properties are those of the tutorial case
* it looks like the wrong smaller temperature was triggering the instabilities due to a bigger density difference between the fresh gas and the burnt one.
Attached Images
File Type: jpg WellerResults.jpg (47.2 KB, 84 views)
File Type: jpg XiFoamInit.jpg (24.6 KB, 91 views)
File Type: jpg XiFoamInitTemperature.jpg (58.3 KB, 80 views)
File Type: jpg XiFoam2_p.jpg (15.4 KB, 76 views)
Attached Files
File Type: txt fvSchemes.txt (2.2 KB, 36 views)
__________________
Frederic Collonval
Technische Universität München
Thermodynamics Dpt.
fcollonv is offline   Reply With Quote

Old   October 7, 2011, 14:38
Default
  #2
Member
 
Hannes Kröger
Join Date: Mar 2009
Location: Rostock, Germany
Posts: 95
Rep Power: 9
hannes is on a distinguished road
Hello Frederic,

I have noticed the same behaviour of the Weller model as you when I simulated this testcase with OF-1.5dev some years ago and I did not find the reason for that.
I have implemented two other combustion models and tested them on the same testcase (same grid and BC's like tutorial case) and they yielded much more physical results.
Take a look here:
http://www.openfoamworkshop.org/08/p...nesKroeger.pdf

Also, I did not succeed in applying the weller model to a partially premixed bunsen flame case. The newton solver for temperature did not converge quite often and also unphysical temperatures occurred.

Regards, Hannes
hannes is offline   Reply With Quote

Old   October 8, 2011, 01:16
Default
  #3
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Since the author of the paper is also one of the developers of OpenFOAM, a report of this issue on mantis ( http://www.openfoam.com/mantisbt/main_page.php ) might give you the answer and eventually a solution.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   October 8, 2011, 03:03
Default
  #4
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
Thanks Hannes and Alberto for the quick answer.

@Hannes: When using the tabulated chemistry, do you read the density from the table? If so, the pressure used in the ideal gas law is the one set in Cantera (presumably 1 atm.) to compute the flamelet, isn't it? You were consequently using a kind of incompressible ideal gas law (as named in Fluent) in which one makes use of the so-called operating pressure independent of the local pressure. Can you confirm that?
For another combustion model, I implemented such incompressible ideal gas law to get rid of numerical acoustic effects as OpenFOAM has no perfectly non-reflecting BC. The improvement was important...

@Alberto: Thank you for the suggestion. I actually thought of it. But I was unsure as it isn't really a bug in OpenFOAM... I will give it a try.
__________________
Frederic Collonval
Technische Universität München
Thermodynamics Dpt.
fcollonv is offline   Reply With Quote

Old   October 8, 2011, 03:06
Default
  #5
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by fcollonv View Post
@Alberto: Thank you for the suggestion. I actually thought of it. But I was unsure as it isn't really a bug in OpenFOAM... I will give it a try.
I don't want to encourage users to report setup problems on bugzilla, but if you can't reproduce a result in the literature using the same model, it might be a bug. In the end, it's better for everyone to have this clarified ;-)
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   October 8, 2011, 03:17
Default
  #6
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
Quote:
In the end, it's better for everyone to have this clarified ;-)
I agree totally
__________________
Frederic Collonval
Technische Universität München
Thermodynamics Dpt.
fcollonv is offline   Reply With Quote

Old   December 30, 2011, 06:58
Default Reply from H. Weller
  #7
Member
 
Frederic Collonval
Join Date: Apr 2009
Location: Technische Universitaet Munich - Lehrstuhl fuer Thermodynamik
Posts: 53
Rep Power: 8
fcollonv is on a distinguished road
Hey guys,

Here is the answer from Henry Weller for the reported bug:

Quote:
I have now spent some time running and re-running this case with numerous combinations of settings, meshes etc. and for much longer than I could afford to do in the mid-90s when I first ran the case and it is indeed problematic. The flame surface instability is VERY sensitive to the setup of the case, the boundary conditions, the numerical schemes, mesh etc. to the point that it is very difficult to use it as a reliable validation case. We will consider alternative cases both for validation and to provide a more reliable tutorial case for XiFoam.
__________________
Frederic Collonval
Technische Universität München
Thermodynamics Dpt.
fcollonv is offline   Reply With Quote

Reply

Tags
rearward step, xifoam

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
Interfoam Droplet under shear test case adona058 OpenFOAM Running, Solving & CFD 3 May 3, 2010 18:46
Porous Media test case Alex FLUENT 0 April 9, 2006 08:23
oscillating airfoil test case Akbar FLUENT 0 July 15, 2005 06:49
Durham test case SAM FLUENT 0 August 16, 2004 05:01
c1 body test case Eric Lenormand Main CFD Forum 0 March 2, 2000 07:54


All times are GMT -4. The time now is 03:50.