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

TwoPhaseEulerFoam convergence problems

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 27, 2008, 11:13
Default Hello every body, First tha
  #61
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9
danielle is on a distinguished road
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
danielle is offline   Reply With Quote

Old   October 27, 2008, 11:52
Default 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
alberto will become famous soon enoughalberto will become famous soon enough
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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   October 27, 2008, 12:20
Default Thanks Alberto, Yes I need s
  #63
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9
danielle is on a distinguished road
Thanks Alberto,
Yes I need some references.
danielle is offline   Reply With Quote

Old   October 27, 2008, 15:18
Default 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
alberto will become famous soon enoughalberto will become famous soon enough
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. 2267-2282, 2008.

- M. T. Dhotre, B. L. Smith, CFD simulation of large-scale bubble plumes: Comparisons against experiments, Chemical Engineering Science
Vol. 62, Issue 23, pp. 6615-6630, 2007.

- S. M. Monahan, R. O. Fox, Effect of model formulation on flow-regime predictions for bubble columns, AIChE Journal, Vol. 53, Issue 1, pp. 9-18, 2006.

- S. M. Monahan, V. S. Vitankar, R. O. Fox, CFD predictions for flow-regime transitions in bubble columns, AIChE Journal, Vol. 51, Issue 7, pp. 1897-1923, 2005.

- N. G. Deen, T. Solberg, B. H. Hjertager, Large eddy simulation of the Gas–Liquid fow in a square cross-sectioned 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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   October 27, 2008, 18:23
Default thanks for your kindness :-)
  #65
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9
danielle is on a distinguished road
thanks for your kindness :-)
I think that I have access to them
danielle is offline   Reply With Quote

Old   October 27, 2008, 20:40
Default 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
alberto will become famous soon enoughalberto will become famous soon enough
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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   October 28, 2008, 20:47
Default Hello every body, when I ret
  #67
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9
danielle is on a distinguished road
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
danielle is offline   Reply With Quote

Old   October 28, 2008, 23:25
Default 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
alberto will become famous soon enoughalberto will become famous soon enough
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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   October 29, 2008, 09:03
Default Hi, Yes yu're true. The e
  #69
Member
 
Danielle PRL
Join Date: Mar 2009
Posts: 42
Rep Power: 9
danielle is on a distinguished road
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.
danielle is offline   Reply With Quote

Old   October 29, 2008, 10:50
Default 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
alberto will become famous soon enoughalberto will become famous soon enough
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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   November 10, 2008, 12:50
Default Dear Alberto, you talked abou
  #71
New Member
 
Rachid bannari
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 12
Rep Power: 9
bannari is on a distinguished road
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
bannari is offline   Reply With Quote

Old   November 10, 2008, 15:04
Default 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
alberto will become famous soon enoughalberto will become famous soon enough
Hi BAN,

the reference is the following:

P. J. Oliveira, R. I. Issa, On the numerical treatment of interphase forces in two-phase 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. 323-360, 1999.

I hope this helps.

P.S. Please, put your e-mail (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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   November 10, 2008, 15:35
Default Thanks, Ok I will make them n
  #73
New Member
 
Rachid bannari
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 12
Rep Power: 9
bannari is on a distinguished road
Thanks,
Ok I will make them now :-)
With kind regards,
bannari is offline   Reply With Quote

Old   November 10, 2008, 18:58
Default Thanks :-)
  #74
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,904
Rep Power: 27
alberto will become famous soon enoughalberto will become famous soon enough
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 open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   June 7, 2016, 05:26
Default
  #75
Member
 
Join Date: Oct 2015
Posts: 48
Rep Power: 2
masoudsh is on a distinguished road
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
masoudsh 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
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


All times are GMT -4. The time now is 02:16.