
[Sponsors] 
Turbulent boundary conditions for bubble column 

LinkBack  Thread Tools  Search this Thread  Display Modes 
October 14, 2005, 00:49 
Turbulent boundary conditions for bubble column

#1 
Guest
Posts: n/a

Dear friends, I am trying to simulate 2D axisymmetric bubble column, operating liquid in Batch mode.I am using ke (dispersed)model to treat the turbulence.I don't have any idea about the turbulent boundary conditions(liquid phase) .Can anyone help me on this issue? Looking forward to ur reply..... Thanks anji


October 14, 2005, 15:37 
Re: Turbulent boundary conditions for bubble colum

#2 
Guest
Posts: n/a

There is no basis for my answer. However, please try using low values. Not 1 (the default) for k and e. Use say for instance, 0.1 for k and 0.25 for e. I repeat, there is no basis for my answer. Only thing I remember is that I saw this in some of the bubble column tutorials.


October 15, 2005, 04:51 
Re: Turbulent boundary conditions for bubble colum

#3 
Guest
Posts: n/a

I really appreciate your suggestion ..I will try simulations with low values of k and e. Actually I am using U(liquid)=0 boundary condition at inlet(batch liquid) and if i use this velocity to calculate k that will become zero..can i use gas velocity to calculate k at inlet? Do u have any idea about tubulent outflow conditions( by nature of problem i will get reverse flow of liquid ) Thanks, anji


October 15, 2005, 09:33 
Re: Turbulent boundary conditions for bubble colum

#4 
Guest
Posts: n/a

The inlet velocity of water is zero. You are correct. When you go the Solve > Initialize > Initialize panel and try to initialize values from inlet, usually Fluent estimates a value of 1 for k and 1 for e to avoid startup trouble. Unfortunately however, even these values do not often work out. Also it will be incorrect to use the gas velocity to estimate inlet values of k and e as the gas moves significantly faster than the liquid when the column is in operation and remember that the k and e that you specify are for the liquid. So try out 0.1 and 0.25 and see what you get. A more practical approach would be to look into experimental data (for example, the liquid velocity profiles) and try to get an estimate for the average liquid velocity and use those to roughly estimate k and e. Well, for the outlet, if you are using a pressure outlet, choose intensity and hydraulic diameter as the turbulence specification method and use a backflow volume fraction of 1 and the hydraulic diameter of corresponding outlet (which for a bubble column is simply the whole diameter of the column (Imp. Note: Just because you are using an axisymmetry boundary condition, you should not assume that the hydraulic diameter is half the column diameter; always input the actual diameter of the column for the hydraulic diameter as this is just a cylinder).


October 15, 2005, 11:46 
Re: Turbulent boundary conditions for bubble colum

#5 
Guest
Posts: n/a

Dear friend, I got the trend of results with <8% differ from literature data.The values mentioned for k and e are working properly for my case.. Thank you very much for ur help..can i get the information regarding tutorials(bubble column) u'he mentioned in the first mail.. thanks


October 15, 2005, 12:19 
Re: Turbulent boundary conditions for bubble colum

#6 
Guest
Posts: n/a

It is nice to know that you are able to predict reasonably good agreement with experimental data. I wish to know however, what parameters have you compared? For instance is it the:
a. Gas velocity profiles b. Liquid velocity profiles c. Gas holdup profiles d. Average gas velocity e. Average liquid velocity f. Average gas holdup Here are some of the tutorials. Note that some of them were prepared for Fluent 4; nevertheless you should be able to understand most of the input easily. 1. (Partially Aerated Bubble Column) http://www.fluentusers.com/fluent45/...tml/node97.htm 2. (Fully Aerated Bubble Column) http://www.fluentusers.com/fluent45/doc/doc_f.htm 3. (Hydrodynamics of Bubble Column Reactors) http://learningcfd.com/login/fluent/...blecolumn.pdf 

October 15, 2005, 12:20 
Re: Turbulent boundary conditions for bubble colum

#7 
Guest
Posts: n/a


October 15, 2005, 23:38 
Re: Turbulent boundary conditions for bubble colum

#8 
Guest
Posts: n/a

I have compared the time averaged profiles of axial liquid velocity and gas holdup...Thanks for sending the links..Actually i am accessing fluent through the institue license so i don't have user name and password to view those tutorials..anyway i will try to get those from our representative...thank u very much anji


October 16, 2005, 01:35 
Re: Turbulent boundary conditions for bubble colum

#9 
Guest
Posts: n/a

In addition to axial liquid velocity and gas holdup I also have to compare the timeaveraged kinetic energy/unit volume(dyne/cm2)..do u have any suggestions to do this? I have written a UDF using ( c_k(c,t)/c_VOLUME(c,t) )..but i have doubt about the units and the volume to be used in the denominator .I am thankful to your continuous help... anji


October 16, 2005, 01:44 
Re: Turbulent boundary conditions for bubble colum

#10 
Guest
Posts: n/a

How can i calculate the turbulent intesity at the outlet?.. Thanks


October 16, 2005, 10:49 
Re: Turbulent boundary conditions for bubble colum

#11 
Guest
Posts: n/a

Use a custom field function:
Define turbulence_intensity as sqrt(2*k/3)/velocity_magnitude_water where 'k' is the turbulent kinetic energy of water. 

October 17, 2005, 05:38 
Re: Turbulent boundary conditions for bubble colum

#12 
Guest
Posts: n/a

Hi, From my knoweldge custom field functions can be used only for intialization(patch) or for plotting the results.I don't know the procedure of using custom feild function as boundary condition.Can u please help with this problem.. Thanks


October 17, 2005, 06:34 
Re: Turbulent boundary conditions for bubble colum

#13 
Guest
Posts: n/a

Hi, Turbulent Intensity is availble in the standard feild functions defined by fluent..so we no need to define it again i think... anji


Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
mesh file for flow over a circular cylinder  Ardalan  Main CFD Forum  7  December 15, 2020 13:06 
Turbulent Boundary Layer on a Flat Plate  Hoshang Garda  FLUENT  1  November 27, 2013 10:24 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 03:32 
Turbulent Boundary Conditions  cfd seeker  FLUENT  2  June 24, 2011 02:28 
Help with boundary conditions  Dan  CFX  0  April 3, 2006 11:32 