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

twoPhaseEulerFoam - sudden enlargement of circular pipe validation case

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 22, 2012, 19:41
Default twoPhaseEulerFoam - sudden enlargement of circular pipe validation case
  #1
New Member
 
Yanxiang Shi
Join Date: Mar 2012
Location: Cambridge, MA, US
Posts: 29
Rep Power: 5
yanxiang is on a distinguished road
Hi all,

In Rusche's thesis, he validated the two-fluid method with the sudden enlargement of circular pipe case. Could anyone send me a copy of this original experimental paper? I can't find it through google or our library.

Bel Fdhila R, Simonin O. Eulerian prediction of a turbulent bubbly ow downstream of a sudden pipe expansion. In Proceedings of the 6th Workshop on Two Phase Flow Predictions, Sommerfeld M (ed), University of Erlangen, 1992)

I followed whatever is available in Rusche's thesis, but I got a high gas fraction zone right after the enlargement (see attachment).

Thanks,
yanxiang
Attached Images
File Type: jpg alpha.jpg (2.8 KB, 47 views)
yanxiang is offline   Reply With Quote

Old   December 23, 2012, 05:09
Default
  #2
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
Are you using the latest 2.1.x code with MULES?
__________________
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   December 23, 2012, 11:55
Default
  #3
New Member
 
Yanxiang Shi
Join Date: Mar 2012
Location: Cambridge, MA, US
Posts: 29
Rep Power: 5
yanxiang is on a distinguished road
Nope. This is OF211. Do you think it would be different if I I use 2.1.x code? Nevertheless, I think, OF211 shouldn't behave like that either.
yanxiang is offline   Reply With Quote

Old   December 24, 2012, 05:42
Default
  #4
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
The MULES version of twoPhaseEulerFoam should do a much better job at ensuring that alpha is bounded, which is less robust in the old version. Maybe give it a try :-)
__________________
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   December 24, 2012, 12:34
Default
  #5
New Member
 
Yanxiang Shi
Join Date: Mar 2012
Location: Cambridge, MA, US
Posts: 29
Rep Power: 5
yanxiang is on a distinguished road
Absolutely. I gave it a try and the result is attached. Gas still tends to go to the corner. The velocity field looks fine though. I have also attached the case tar ball for your review.

Thanks,
yanxiang
Attached Images
File Type: jpg tPEF21x.jpg (41.8 KB, 48 views)
Attached Files
File Type: gz suddenExpansion.tar.gz (3.5 KB, 29 views)
yanxiang is offline   Reply With Quote

Old   December 24, 2012, 23:59
Default
  #6
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 675
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by alberto View Post
The MULES version of twoPhaseEulerFoam should do a much better job at ensuring that alpha is bounded, which is less robust in the old version. Maybe give it a try :-)
Sorry for hijacking this thread.But I really need you help,Prof.Alberto.
Much details has been depicted here
bubblefoam totally failed on unstructured mesh.

Look forward to you replay.Thanks in advance.
sharonyue is offline   Reply With Quote

Old   December 26, 2012, 09:36
Default
  #7
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 yanxiang View Post
Absolutely. I gave it a try and the result is attached. Gas still tends to go to the corner. The velocity field looks fine though. I have also attached the case tar ball for your review.

Thanks,
yanxiang
I don't see problems in the setup of your case. The accumulation of gas in the corner does not seem too different from Rusche's results (Fig. 3.3 c, page 131).

It is possible you have less numerical diffusion than in those results (it seems so from your picture). You should run with the same schemes to have an apple to apple comparison.

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   December 26, 2012, 10:07
Default
  #8
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 sharonyue View Post
Sorry for hijacking this thread.But I really need you help,Prof.Alberto.
Much details has been depicted here
bubblefoam totally failed on unstructured mesh.

Look forward to you replay.Thanks in advance.
I commented on the other thread.
__________________
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   January 2, 2013, 12:39
Default
  #9
New Member
 
Yanxiang Shi
Join Date: Mar 2012
Location: Cambridge, MA, US
Posts: 29
Rep Power: 5
yanxiang is on a distinguished road
Hi Alberto,

I tried the same schemes as used by Rusche, but the results stay pretty much unchanged, with a high gas zone in the corner, and this is not there in Rusche's results, or in Oliveira's (Int. J. Numer. Meth. Fluids 2003; 43:1177–1198). I played around with the BC's, but still couldn't get rid of that. Also, sadly, I was not able to find any of the references (except for Oliveira's) used by Rusche in that particular test case section where others validated their models with it. Do you have any of those papers?

Thanks,
Yanxiang

P.S: Happy New Year!!!!
yanxiang is offline   Reply With Quote

Old   January 2, 2013, 12:50
Default
  #10
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
How did you decide the BC's for the turbulent quantities? They aren't provided in the article...
__________________
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   January 2, 2013, 13:22
Default
  #11
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
I ran the case you attached turning turbulence off, just to see the effect, and segregation is much lower, as expected.

Anyways, I am working on a validation case for twoPhaseEulerFoam/multiphaseEulerFoam for bubbly flows... we'll see :-)
Attached Images
File Type: jpg alpha1.0012.jpg (10.1 KB, 28 views)
__________________
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   January 2, 2013, 16:18
Default
  #12
New Member
 
Yanxiang Shi
Join Date: Mar 2012
Location: Cambridge, MA, US
Posts: 29
Rep Power: 5
yanxiang is on a distinguished road
Alberto,

So after reading your question about the turbulent quantities, I made some changes to my very original test case at work, and ran the OF211 version of tPEF on it. Weirdly, it worked :-$. By that I mean, I got similar results to those in Rusche's and Oliveira's works. I will try to reproduce that with OF21x version when I get home (although a diff on the two cases didn't give me any hints why the results would differ). Anyways, I attached the screenshots and case for OF211.

Best,
yanxiang
Attached Images
File Type: jpg alpha.jpg (11.7 KB, 31 views)
File Type: jpg k.jpg (10.6 KB, 28 views)
File Type: jpg nut.jpg (12.1 KB, 28 views)
Attached Files
File Type: gz suddenExpansion.tar.gz (3.5 KB, 20 views)
yanxiang is offline   Reply With Quote

Old   January 2, 2013, 17:18
Default
  #13
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
There is a significant difference in the two algorithms used to solve for alpha in twoPhaseEulerFoam before and after the introduction of MULES, which might explain the differences. I am running some validation cases exactly to see if accuracy was maintained (for now, it is, at least in the case of a simple bubble column).
__________________
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   January 2, 2013, 20:01
Default
  #14
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 675
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by alberto View Post

Anyways, I am working on a validation case for twoPhaseEulerFoam/multiphaseEulerFoam for bubbly flows... we'll see :-)
I am eager to see validation cases for twoPhaseEulerFoam on tet mesh~
sharonyue is offline   Reply With Quote

Old   January 2, 2013, 21:06
Default
  #15
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 sharonyue View Post
I am eager to see validation cases for twoPhaseEulerFoam on tet mesh~
I am not considering tetrahedral grids, because my geometry does not require them (it is a box with rectangular section!). I consider this test-case because it is the precursor for new model developments.

If you want to perform a verification and validation study on tetrahedral meshes, however, it should not be that hard. You should consider a simple geometry with well-defined results (there are many on bubble columns in the literature, pick a case where simulation results are also available, and check the model is the same), do a grid-independence study, and then do the experimental validation on the converged grid.

P.S. Have you tried to use more appropriate numerical schemes, as I suggested in the other thread, with a good quality mesh?
__________________
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   January 2, 2013, 22:04
Default
  #16
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 675
Rep Power: 8
sharonyue is on a distinguished road
Quote:
Originally Posted by alberto View Post
I am not considering tetrahedral grids, because my geometry does not require them (it is a box with rectangular section!). I consider this test-case because it is the precursor for new model developments.

If you want to perform a verification and validation study on tetrahedral meshes, however, it should not be that hard. You should consider a simple geometry with well-defined results (there are many on bubble columns in the literature, pick a case where simulation results are also available, and check the model is the same), do a grid-independence study, and then do the experimental validation on the converged grid.

P.S. Have you tried to use more appropriate numerical schemes, as I suggested in the other thread, with a good quality mesh?

I am sorry about that question. because it looks like there is no substantial change to the result.but I dont know if its still because of the mesh.


So I refine the mesh, now the cell is half than that cell in the other thread.so the total cell number reachs to 1,79 million,its too many, so I shorten the height, the other thing is not changed.the total cells number is about 55000.

I attached my image.I think that dont need to depict it.My primary language is not english so~.

btw,I turn to the other thread,I am sorry for that.
bubblefoam totally failed on unstructured mesh.

Thanks for you consistent attention.Alberto
Attached Images
File Type: jpg 1.jpg (22.2 KB, 18 views)
File Type: jpg 2.jpg (76.8 KB, 12 views)
File Type: jpg 3.jpg (35.5 KB, 11 views)
File Type: jpg 4.jpg (30.6 KB, 10 views)
File Type: jpg 5.jpg (31.9 KB, 11 views)
sharonyue is offline   Reply With Quote

Old   January 4, 2013, 00:22
Default
  #17
New Member
 
Yanxiang Shi
Join Date: Mar 2012
Location: Cambridge, MA, US
Posts: 29
Rep Power: 5
yanxiang is on a distinguished road
Hmmm... interesting. I tried the OF21x version on the same case again, and as you would expect, the results just look like what we had previously. So does that mean the new solver with the MULES method is not solving the alpha equations correctly?

Thanks,
yanxiang
yanxiang is offline   Reply With Quote

Reply

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
Validation of circular pipe flow with/without square edged orifice plate Gamb1t Main CFD Forum 0 December 27, 2011 11:56
Laminar Circular pipe flow problem GLee CFX 6 September 15, 2011 10:57
Turbulent Flat Plate Validation Case Jonas Larsson Main CFD Forum 0 April 2, 2004 10:25
+ shape circular pipe - meshing possible? Selina Tracy Main CFD Forum 2 January 16, 2003 14:31
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 20:21.