[danielle]

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

[alberto]

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

[danielle]

Thanks Alberto,
Yes I need some references.

[alberto]

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

[danielle]

thanks for your kindness :-)
I think that I have access to them

[alberto]

You're welcome!

[danielle]

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

[alberto]

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

[danielle]

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.

[alberto]

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.

[bannari]

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

[alberto]

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

[bannari]

Thanks,
Ok I will make them now :-)
With kind regards,

[alberto]

Thanks :-)

[masoudsh]

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