
[Sponsors] 
October 27, 2008, 11:13 
Hello every body,
First tha

#61 
Member
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9 
Hello every body,
First thank you for your help. My problem is not where I should put the diametres of phase a and b. I have a reator which initaly has a half full with water, the other half is filled with air. I inject only the air. I think in that case dragPhase is blended. my problem is the value which I should give to db. This value will influence strongly the drag. Thanks 

October 27, 2008, 11:52 
Hi Danielle,
I think you can

#62 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hi Danielle,
I think you can use a "standard" drag law without blending, so that you need to specify only the mean bubble diameter, as done in many papers regarding bubble column simulations. Corrections to the the traditional drag laws are done for example to account for bubble deformation, but this has nothing to do with using a "blended" formulation, which looks quite artificial to me. If you need references to the literature on the topic, feel free to ask. Regards, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

October 27, 2008, 12:20 
Thanks Alberto,
Yes I need s

#63 
Member
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9 
Thanks Alberto,
Yes I need some references. 

October 27, 2008, 15:18 
Hi Danielle,
I report some

#64 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hi Danielle,
I report some references (have you access to them?) taken from the recent literature about bubble column simulations. As you can see from the titles, they deal with various topics, however all these papers clarify the adopted drag law. If you need more information, don't hesitate to ask. :)  M.R. Bholea, J.B. Joshia, D. Ramkrishna, CFD simulation of bubble columns incorporating population balance modeling, Chemical Engineering Science, Vol. 63, Issue 8, pp. 22672282, 2008.  M. T. Dhotre, B. L. Smith, CFD simulation of largescale bubble plumes: Comparisons against experiments, Chemical Engineering Science Vol. 62, Issue 23, pp. 66156630, 2007.  S. M. Monahan, R. O. Fox, Effect of model formulation on flowregime predictions for bubble columns, AIChE Journal, Vol. 53, Issue 1, pp. 918, 2006.  S. M. Monahan, V. S. Vitankar, R. O. Fox, CFD predictions for flowregime transitions in bubble columns, AIChE Journal, Vol. 51, Issue 7, pp. 18971923, 2005.  N. G. Deen, T. Solberg, B. H. Hjertager, Large eddy simulation of the Gas–Liquid fow in a square crosssectioned bubble column, Chemical Engineering Science, Volume 56, pp. 6341–6349, 2001. With kind regards, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

October 27, 2008, 18:23 
thanks for your kindness :)

#65 
Member
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9 
thanks for your kindness :)
I think that I have access to them 

October 27, 2008, 20:40 
You're welcome! http://www.cfd

#66 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
You're welcome!
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

October 28, 2008, 20:47 
Hello every body,
when I ret

#67 
Member
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9 
Hello every body,
when I retransferred the explecit drag from the p equation to the U equation (the original form for the momentum equation) I get unrealistic result ! I added: (beta/rhoa*K*Ub) and (alpha/rhob*K*Ua) to UaEq and Ubeq. and I remove (fvc::interpolate(alpha/rhob*K*rUbA)*phia) and (fvc::interpolate(beta/rhoa*K*rUaA)*phib ) from phiDragb and phiDraga. what you think about this ? NB: It's important to me to write this drag term in Ua and Ub Eq. thanks for help 

October 28, 2008, 23:25 
Hi Danielle,
what do you me

#68 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hi Danielle,
what do you mean with "unrealistic results"? A completely explicit drag treatment is known to be slowly converging when a high drag coefficient is present. And actually only partial elimination and coupled solution of the equations are known to converge on a wide range of flow conditions (see for example the work of Oliveira and Issa). May I ask why do you need a fully explicit treatment? :) Moreover, using a fully explicit treatment, your time step is not limited only by the Courant number, but also by the drag time. In these cases it is common practice to use the minimum time step determined on the basis of the Courant number for each phase and the drag time divided (usually) by 10. This of course will slow down the calculation quite a bit. Regards, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

October 29, 2008, 09:03 
Hi,
Yes yu're true. The e

#69 
Member
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9 
Hi,
Yes yu're true. The explicit drag is very slow in convergence, when I use the original form (in p equation) I get a good result with experimental, but with the explicit form the volume fraction still unchanged from the initial form until 120s of simulation! Why I will write a fully explicit treatment? I try to implement the MRF in this solver. When I use the explicit form with the flux correction (like MRFSimpleFoam) for phia and phib I get a good result for the velocites, but the volume fraction still unchanged (the air don't move up from inlet). with the original form the correction of flux give the velocities 4 times greater that I must get. 

October 29, 2008, 10:50 
Hi Danielle,
it seems to me

#70 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hi Danielle,
it seems to me your simulation is not actually converging. What time step are you using? Keep in mind of the need to account for the drag time in the calculation of the time step with the explicit treatment. Regards, A.
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 10, 2008, 12:50 
Dear Alberto,
you talked abou

#71 
New Member
Rachid bannari
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 12
Rep Power: 9 
Dear Alberto,
you talked about the work of Oliveira and Issa about the partial implicit form for drag treatment. which one ? I need this reference. Thanks 

November 10, 2008, 15:04 
Hi BAN,
the reference is th

#72 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Hi BAN,
the reference is the following: P. J. Oliveira, R. I. Issa, On the numerical treatment of interphase forces in twophase flow, Numerical Methods in Multiphase Flows, Vol 185, ASME, 1994. You might also be interested in H. Karema, S. Lo, Efficiency of interphase coupling algorithms in fluidized bed conditions, Computer & Fluids, 28, pp. 323360, 1999. I hope this helps. P.S. Please, put your email (and possibly your name) in the profile. I won't answer to questions of people without that anymore from now on. Don't take it personal, of course, you are not alone and it is not referred only to you for sure. I am simply taking advantage of your question to point out an old problem. :) With kind regards, Alberto
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

November 10, 2008, 15:35 
Thanks,
Ok I will make them n

#73 
New Member
Rachid bannari
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 12
Rep Power: 9 
Thanks,
Ok I will make them now :) With kind regards, 

November 10, 2008, 18:58 
Thanks :)

#74 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27 
Thanks :)
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 7, 2016, 05:26 

#75 
Member
Join Date: Oct 2015
Posts: 48
Rep Power: 2 
Hi Alberto
I spent a long time for simulation with towphasEulerFoam I initially met by reducing the time, then a significant increase Epsilon And also decrease over time step I've changed my mesh And now I'm faced with another problem Alpha is the negative resolution http://www.uupload.ir/files/dq5e_595...06a70c0a99.png Do you know the reason? Thanks 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Some problems with twoPhaseEulerFoam  su_junwei  OpenFOAM Running, Solving & CFD  2  November 2, 2012 02:12 
Convergence problems!!  Elleana  FLUENT  9  June 10, 2008 04:39 
Convergence problems  please help  M Liddell  FLUENT  3  February 8, 2005 20:06 
convergence problems  jeremy  FLUENT  7  May 30, 2002 06:41 
Convergence Problems  Prateep Chatterjee  FLUENT  7  October 9, 2001 09:29 