Dear,

I am trying to simulate a Bubble Column, a 2-D model to start with. For the bubble injection at the bottom, with Bubble diameter like 2 mm, 1. Is it better to define some cells at the bottom as air inlet, while others as wall boundary condition, or should I define the whole bottom as air inlet? 2. Should I check the option for "Specified Operating Density" for the Operating conditions? 3. Which model for the multiphase model is the most suitable?

Any suggestion is welcome.

1) Just choose the geometry configuration on the basis of the real system you want to simulate.

2) Yes, check the Specified Operating Condition option if you want to include gravity effects.

3) I'd suggest the Eulerian Multiphase Model.

If you want to capture the plume oscillation frequency, you had better to do a 3D calculation, using an high order discretization scheme (Second order, o QUICK).

Hi

ap

Hi, 1 - the whole inlet has to be air inlet. Defining the grid in your geometry will required to use the VOF model which only make sens if you want to model what happen only what happen above the grid in a small domain. Also concerning the other multiphase model (mixture, euler euler, DPM) you already define the bubble diameter in your setup, therefore you do not need to define a grid.

2- it is always good to turn on the 'Specified Operating Density' option.

3 - I would say it depends on your flow regime and air volume fraction. -Mixture model fits with homogeous model (Low volume fraction, low velocity in general, small bubble) -Euler-euler model fits with the other cases.

My personal advice is to use the euler euler model. Some people will certainly tell you it will take longer time to converge, but considering the case of a simple bubble column I do not think it is gonna be significant.

hope this help thomas

Hello, thomas, what is the mean of grid you mentioned?is it necessary and important for simulating two phase flow? and if necessary, how to define it? and i don't know what you say in your first paragraph,would you like to explain it for me further plain? thanks in advance.

Sorry, I misunderstood the first question, about which I agree with thomas.

Hi

ap

Hi,

Thanks for the response. (1) One of my basic misconceptions: Defining the whole bottom plate as the air inlet: What would it mean physically? What I have tried after ur suggestion is: to define that as a velocity inlet, phase: air, and air phase fraction: 1. But would it approximate a sparger, because in a physical bubble column, most of the bottom plate is to be like a a stationary wall, and only the sparger holes would be the air inlets? (2) When I turn on the specified operating density, it needs me to specify an operating density, but what does an operationg density mean? Because the bubble column density would be varying depending on the phase distribution. (3) This part is clear to me now. (4) If I want to visualize the phase distribution, at steady state, which one would u think is better: To turn on the steady steady state option, or to use the unsteady state model, and stop when the solution does not change any further? I used the steady state option, and as u suggested the Eulerian multiphase model, but the problem did not converge, or the residual plots don't suggest that it will converge at all. (5) What I understand is to start with an initial condition with air phase fraction of zero (full of water) and based on the air superficial velocity and gravity, we will get a plume distribution in the bubble column liquid at steady state. Or is it that steady state solution won't be possible at all, since the plume would be oscillatory in nature?

Thanks a lot

Hello,

Thanks for the response. (1) One of my basic misconceptions: Defining the whole bottom plate as the air inlet: What would it mean physically? What I have tried after ur suggestion is: to define that as a velocity inlet, phase: air, and air phase fraction: 1. But would it approximate a sparger, because in a physical bubble column, most of the bottom plate is to be like a a stationary wall, and only the sparger holes would be the air inlets? (2) When I turn on the specified operating density, it needs me to specify an operating density, but what does an operationg density mean? Because the bubble column density would be varying depending on the phase distribution. (3) This part is clear to me now. (4) If I want to visualize the phase distribution, at steady state, which one would u think is better: To turn on the steady steady state option, or to use the unsteady state model, and stop when the solution does not change any further? I used the steady state option, and as u suggested the Eulerian multiphase model, but the problem did not converge, or the residual plots don't suggest that it will converge at all. (5) What I understand is to start with an initial condition with air phase fraction of zero (full of water) and based on the air superficial velocity and gravity, we will get a plume distribution in the bubble column liquid at steady state. Or is it that steady state solution won't be possible at all, since the plume would be oscillatory in nature?

Thanks a lot

Hi, I understand the difficulty about taking into account or not the grid geometry. For my little personal story I needed a certain time before completely I figured that out. I will try to make it simpler.

A – Grid/sparger ? I am gonna try to make it very simple.

1 - What is the aim of a grid/sparger in bubble columns? -> Creating the bubble at inlet. We all know the bubble diameter mainly depends on the grid hole diameter.

2 - Do we need to take into account the grid? -> The answer is no cause we already defined a bubble diameter using the Eulerian model. Therefore defining the grid becomes useless!

3 – Influence on velocity without taking into account the grid? None, only if the velocity set at the inlet is the superficial velocity (the data is known in general).

4 – How taking into account the fact it exists different type of grid/sparger? Well here is the problem. Of course if your bubble column is locally aerated by only one small inlet it is obvious that you do have to create an inlet geometry with one small hole. In other cases the approximation is that the grid influence is not significant after a certain height (which is of course not that simple in reality). For further informations on that just consult a researcher or check for example the publication Hills (1974) 'Radial non uniformity of velocity and voidage in b. c.'

B – How about operationg density ? I have personally not understood yet what is it. Go to see what is it said on the fluent documentation (I have not looked at it yet). Check older questions on the cfd-online forum. Also what do you mean by ' ... Because the bubble column density would be varying depending on the phase distribution … ' ???

C – Steady state ? On a instantaneous point of view it is NOT a steady state because the air plume can be considered as oscillating in reality. However in 2D simulation you force your hydrodynamics to achieve a steady state. Now what a lot of paper says is it is better to simulate the column 'unsteady' (with a time step). Personally I did not succeed to achieve a converged result with steady state simulation.

Hope that informations will help ya. Tom.

PS : Est-ce qu'ils connaissent le PSG en suède ?

1) In my first answer I told you to create the grid according to the real geometry. I meant you have to define as inlet only the portion of the botton of your column which really is the inlet, not the whole bottom plate, like in the following scheme.



| |
| |
| wall |
| / \ |
----| |----

\_ Inlet



Obviously, as said by thomas, you don't need to define the sparger on the inlet, because you've already set bubble diameter in the phase panel.

2) You can find the answer in FLUENT manual.

4) Your system is not steady, so you should do unsteady calculation. You don't obtain a converged solution using the steady solver because the steady model isn't able to properly represent what happens in your system.

5) The plume is oscillatory. You can find many works in literature which explains this and gives information on how to simulate bubble columns.

For example in: F. Bertola, M. Vanni, and G. Baldi (2003) "Application of Computational Fluid Dynamics to Multiphase Flow in Bubble Columns," International Journal of Chemical Reactor Engineering, Vol. 1: A3.
http://www.bepress.com/ijcre/vol1/A3, you can find a comparisons between results obtained usign FLUENT and CFDLIB, with indications on discretization schemes, grids and model options.

Hi

ap

Thanks for the valuable suggestions, Tom. When I said ' ... Because the bubble column density would be varying depending on the phase distribution … ', I meant that because of the phase (of different densities) distribution in the bubble column volume, there will also be a density distribution, and a single density will not exist. So when I turn on the "Specified Operating Density", and mention an operating density, what will that imply?

Is this for a school project or an industrial one?

thomas

Yes,

This is for a Masters Thesis project. Thanks a lot again.

What are the thing you are looking for in your bubble column ? just a simple simulation or you are trying to reproduce publication results ?

thomas

Well, for the time being it is just an effort to reproduce publication results or validate some published experimental data, which might help us to make further investigations on sparger design etc. Can you suggest some important directions for my Masters project? Thanks in advance.

please see my first leave word, it is for you

[yuvarajp]

hi im trying to simulate my bubble column ith initial liquid heightas 3m and overall height is 5m. how can i model this in fluent. i made my mesh for 5m and have to specify my liquid height now. i would appreciate ur help.