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

twoPhaseEulerFoam - test case validation

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

Like Tree1Likes
  • 1 Post By GerhardHolzinger

Reply
 
LinkBack Thread Tools Display Modes
Old   December 17, 2013, 09:49
Default twoPhaseEulerFoam - test case validation
  #1
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
Hello everyone,

I'm working with the solver "twoPhaseEulerFoam", trying to reproduce the results shown in "Numerical simulation of the dynamic flowbehavior in a bubble column: A study of closures for turbulence and interface forces" by D. Zhang, N.G. Deen∗, J.A.M. Kuipers.

Did anyone already work on that topic ?

I have have test several parameters (mesh size, time step, void fraction at the inlet, lift force coefficient...) but so far I'm not able to reproduce the results in terms of the dispersed phase velocity and the continuous phase velocity.

If anyone is working on this, I'd be pleased to share any tips/work.
Aurelien Thinat is offline   Reply With Quote

Old   December 19, 2013, 04:49
Default
  #2
Senior Member
 
Gerhard Holzinger
Join Date: Feb 2012
Location: Austria
Posts: 166
Rep Power: 14
GerhardHolzinger will become famous soon enoughGerhardHolzinger will become famous soon enough
Hi,

I followed the paper of Deen, Solberg and Hjertager of 2001 (Large eddy simulation of the Gas–Liquid ow in a square cross-sectioned bubble column)

There the same geometry is used. In order to do this simulations I had to extend the standard drag models (e.g. the Ishii-Zuber drag model) and I had to modify twoPhaseEulerFoam to make use of the generic turbulence models, in order to use LES turbulence. The k-eps turbulence model tends to establish a dominant vortex in the domain.

The mesh consists of 3 times 3 blocks. The top surface is modelled with a slip BC for the water. I had to set the inlet volume fraction to 0.6 in order to get a well behaving simulation. Consequenty, the inlet velocity has to be higher in order to match the volumetric gas flow rate.

The mesh fineness is limited by the Milelli condition. It says that the cell size should not be smaller than the bubble size. [A numerical analysis of confined turbulent bubble plumes, Massimo Milelli, PhD thesis, 2002]

One of the findings of Deen et al. was that the lift force is essential to match the measured profiles. My results also led me to that conclusion. In the attached images you see a case with drag, lift and virtual mass (case1) and a case with only drag as interfacial momentum exchange term (case4).

To initialize the simulation I run it with a fixed time step of 0.001 s for 10s, then I switch to variable time stepping and I activate the field averaging function object. Deen uses the averaged field values of the last 140s of the simulation. So, I ran the simulation for 140s after the initialisation.
Attached Images
File Type: jpg case01alphaIsoVolume04U2vectorsT160.jpg (28.4 KB, 83 views)
File Type: jpg case04alphaIsoVolume04U2vectorsT160.jpg (23.8 KB, 80 views)
davibarreira likes this.
GerhardHolzinger is offline   Reply With Quote

Old   December 19, 2013, 12:57
Default
  #3
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
Hi Gerhard,

Thank you for your answer.

I have a question regarding the use of LES in such cases. When the bubble's diameter is greater than 1 mm, considering the Milelli condition, does it make any sense for a LES computation ?

In the Zhang's publication I mentionned, they are working with bubbles of size of 0.004 meter in a square-section cylinder of 0.15x0.15 m² area. That seems to be really huge cells compared to the volume of fluid.
Aurelien Thinat is offline   Reply With Quote

Old   December 19, 2013, 13:03
Default
  #4
Senior Member
 
Gerhard Holzinger
Join Date: Feb 2012
Location: Austria
Posts: 166
Rep Power: 14
GerhardHolzinger will become famous soon enoughGerhardHolzinger will become famous soon enough
Hi,

I am no expert on LES. However, using LES seems to work better than using kEpsilon.

The difference between VOF and Eulerian multiphase simulations is that in the Eulerian simulation you assume that the gas phase is dispersed in the liquid phase. If you further assume that your control volumes are larger than the bubbles you can treat the gas phase as a continuum. And that's were the Milelli condition comes in.

In VOF you want to resolve the surface that separates gas from liquid. That's why you need fine cells there.

That's all I can say besides, it works if you use LES.


Cheers
GerhardHolzinger is offline   Reply With Quote

Old   April 27, 2014, 17:38
Default
  #5
aka
New Member
 
Getnet
Join Date: Aug 2011
Location: LSU
Posts: 20
Rep Power: 6
aka is on a distinguished road
Is there anyone out there who has done a horizontal channel/pipe test with twoPhaseEulerFoam? I am planning to use this solver for conditions where shear is important.

Thanks,
Getnet
aka 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
twoPhaseEulerFoam - sudden enlargement of circular pipe validation case yanxiang OpenFOAM Running, Solving & CFD 16 January 4, 2013 00:22
CFX-Pre problem, pls help!!! cth_yao CFX 0 February 17, 2012 01:52
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24
Combustion Test Case A.S. Main CFD Forum 1 May 31, 2005 09:22
Heat Transfer Validation test case Chris Whitney Main CFD Forum 1 July 21, 1999 14:36


All times are GMT -4. The time now is 15:58.