Hi, I am trying to model the 2-D flow dyanmics of bubble column (gas-liquid flow) using FLUENT, however, I do not get right profile result of the Gas Hold-Up (Gas Volume Fraction). I am trying to work on the Half Domain model because the bubble column is a symmetric geometry with respect to the centerline.

Could anyone suggest the right B.C. to model the bubble column for me? Also, how do you really model gas-liquid flow in Bubble Column? ( I don't see FLUENT tut. manual providing any bubble column modeling), Thanks.

I appreciate your help.

dlaw

Hi dlaw,

Modeling bubble column in axisymmetry geometry is not a good idea even the geometry is symmetric w.r.t the centerline because the fluid flow sometimes varies along the axis.

Use velocity inlet for inlet, and pressure outlet B.C for the outlet. You could patch a vof of 1 for gas at the top section so that the gas-liquid interface rises as gas is sparged into the column.

There are two tutorial's in fluent's multiphase flow application tutorials..follow the link http://www.learningcfd.com/login/flu...ials/index.htm

I hope this helps,

aPpA

Hi aPpA, which turbulence model (two fluid Eulerian) you use for bubble column multiphase flow under churn-turbulent flow regime? There are three turb. model options in FLUENT such as Mixture, Dispersed, and Per Phase models. Also, which drag function do you use as well? It seems to me that Morsi-Alexander and Symmetric both can be used for bubble column gas-liquid flow modelling.

Thanks for your reply and help.

dlaw

As far as turbulence model goes the most app. model would be dispersed. Refer to the paper by Davour Cockljat in ASME series. It uses k-e in continuous phase and T Chens theory for dispersed phase. You can also enable dispersion in this case. The sucess of bubble column or to make it general G-L simulations comes from the fact that: 1. Closure is handled correctly and let me tell you experience shows different drag laws does not play a big role till you are working with higher holdup. 2. Free surface boundary conditions at outlet should be used/ tested. 3. Turbulent dispersion should also be used. 4.Lift can cause instabilities in ur case. 5. Try virtual mass as I am stumbling on it and not sure. PS: If u are concerned with drag laws use Ishii and Zuber (1979) as its better than many, however Schiller and Naumann (1935) does the same. Another piece of advise G-L problems are complex to work with hence beign patient really helps.

Hi Podila, when I used Dispersed Turbulence Model, FLUENT tends to give me "Reversed flow at the outlet" message. Also, I am not able to use Pressure Outlet boundary condition at outlet with Dispersed Turb. Model. However, I don't encounter with the reversed flow and outlet condition problems by using Mixture Turb. Model.

For some reasons, I still get the same Mean Gas Volume Fraction results with both Mixture and Dispersed Turb. Models. I need your enlightenment in this regard. Thanks. I appreciate your help.

Bubble columns will have flow reversal. The reason is pretty simple as the water will not leave the columns and hence will be recirculated.This implies flow reversal. Do u want the water to leave the column? I think not... But still flow reversal is caused due to the fact that u are not having a good grid. What is your wall Y+. Are u checking on area weighted average??????? for the gas holdup. Which domain u are looking for avg.???

This is vague. U can use pressure outlet. The place where u are going wrong is in GAMBIT. U are not checking on FLUENT while exporting mesh and hence those option are not highlighted to you when you are exporting mesh. Hence I would advise look through the mesh and check FLUENT option in solver... While exporting also check on export 2D mesh. "For some reasons, I still get the same Mean Gas Volume Fraction results with both Mixture and Dispersed Turb. Models. I need your enlightenment in this regard" Then there is no difference between the prediction of models and your conclusion is that mixture and dispersed model predict same results. BUT THIS IS UNLIKELY...CHECK ON TURBULENCE INTENSITY FOR CONTINUOUS PHASE.

Hi Podila, I got it to work. However, how to get rid of the "Turbulent viscosity limited to viscosity ratio of 1e+5 in certain number of cells" message during the iteration. The reversed flow message is gone but the "turbulent viscosity......" still remains.

Also, could you simulate a Half Domain G-L flow ( model with respect to centerline of axissymmetric geometry) successfully with FLUENT? That way, the simulation time can be shorter.

I really appreciate your help.

dlaw

One should not use symmetry for bubble column. Physics does not allow to do so. Check your grid and let me know what the wall Y+ you are in?.

HI Podila, How do you get wall Y+ from Fluent? Please let me know the way to extract this wall Y+ in detail. Thanks.

report--->Area weighted average--->Turbulence---->WallY+--->Water Select Wall

Wall Y+ is key to turbulent flow simualtions. Read more about that in manuals and research papers.

For some reason, I don't see Area Weighted Average under Report section in FLUENT 6.1 version.

I found that the "Turbulent viscosity...." message is very sensitive to the Cell Size, which means it will disappear the message if I change to a different Cell Size.

I am not sure why u did not finad the option of are weighted average.Good luck

Hi Podila, which discretization scheme (Power Law, Second order upwind, Quick) do you use to simulate bubble column gas-liquid flow.

dlaw

Do a simple run which one works best for you. I run the deafult which is upwind if I am correct.

I used Eulerian Dispersed turbulence model, Morsi-Alexander Drag model, and Power Law(basically I follow whatever you said in the previous messages) to run the simulation; however, I still do not get the right Time-Averaged gas volume fraction profile results, which should have the largest gas volume fraction at the center of the bubble column and decrease as it approaches the wall of buble column. The profile should look like an inverted quadratic curve. I hope you understand what I said here. I also input gas volume fraction=1.0 at the velocity inlet boundary due to gas is the secondary phase here. Do you know what else goes wrong regarding the inaccurate time-averaged gas volume fraction profile?

Thanks and I really appreciate your help thus far and in advance.

There is nothing going wrong in your problem set up but you are missing to account for turbulent dispersion force which smoothes the profile by spreading the gas volume fraction uniformily through the domain. Various models of dipsersion are present which one can customise via UDF's. Could u send me the simualted curve with experimental ata on it so that I can discuss more on this issue. I would suggest try to increase and decrease the bubble diameter and see what happens and then one can also play with constnats in k-e model but thats far sighted. First u have to account for the momentum transfer funtions accurately which are drag, lift and dispersion. In your case lift does not play a huge role except at high gas velocities but drag and dispersion go hand in hand. I would reccommend a drag function of Ishhi and Zuber in cap bubbly flow regime which is independent of bubble diameter.

Dispersion forces of higher magnitude have to be used. DId u try with other turbulence models. Which turbulent model u are using. I suggest and reccomend only dispersed phase turbulent model to be used. Please also enable the source terms (Enable momentum trnasfer). This can be done using Define-Models_viscous_Mutliphase_enable momentum. "Send me the graph and then we can discuss in detail"

[SITD]

Hi,
I encountered some problems during a similar bubble column project. If you can recall the works you've done (since it very long time back), will you be able to help me out?
Thanks in advance

Regards
SITD

[thanhvn]

Hi. I have the same problem. Can you help me this work? my email leminhthanhth@gmail.com
Thanks.

[azna]

Hi ,
I need to simulate a bubble column with Eulerian model in Fluent, However I don't know how can I define bubble sizes between 3 to 4 mm instead of a constant bubble size ? in the phases there is a option to define bubble diameter but it's only for constant value .

Thanks