First, did you try 2 phase solution without PBM? Add complexity in steps, first familiarize yourself with multi-phase before moving to the really complex problems.

Then, to add pbm, you have to load the PBM model via /define/models/addon-module

It will now pop up as an option under your models tab. There, select formulation (QMOM or class-based). My personal experience is that the QMOM model as provided in FLUENT is a bit more unstable, but both give reasonable results. The local BSD is more easy to reconstruct from classes, but if you are only interested in Sauter mean, QMOM is likely faster (although not many classes are needed in bubble flow, so the difference is minor). Then choose breakup/coalescence. Quite frankly I think the only option here is to go for Luo or user-defined functions. There are many other options mainly for break-up, but the problem is the exact rates can differ quite widely between formulations (see e.g. Wang et al 2005) and hence using a breakup and coalescence model by different authors with different underlying principles (and fitting parameters) seems erroneous to me. However, considering literature, Wang's or Lehr's model is likely more accurate - I hope future versions will include these for coalescence, too (or if someone has a UDF implementation, if you could share it...)

With models selected, set boundary conditions. you will need to supply at least classes/moments at all inlets, and probably also at outlets for possible backflow. It's also good to use patch to fix an initial bubble size in the entire domain (I typically just put everything in one class there, between 2 and 5 mm depending on expected outcome). Then run. Higher order schemes may be problematic, start with first order and see if you can go better afterwards.

Good luck!

Have you ever tried two options known as PATCH/UDF?

Hi Yasin,

I know about the PATCH, but have never used it. Are you working on the stirred tank reactors.

First, did you try 2 phase solution without PBM? Add complexity in steps, first familiarize yourself with multi-phase before moving to the really complex problems.

Then, to add pbm, you have to load the PBM model via /define/models/addon-module

It will now pop up as an option under your models tab. There, select formulation (QMOM or class-based). My personal experience is that the QMOM model as provided in FLUENT is a bit more unstable, but both give reasonable results. The local BSD is more easy to reconstruct from classes, but if you are only interested in Sauter mean, QMOM is likely faster (although not many classes are needed in bubble flow, so the difference is minor). Then choose breakup/coalescence. Quite frankly I think the only option here is to go for Luo or user-defined functions. There are many other options mainly for break-up, but the problem is the exact rates can differ quite widely between formulations (see e.g. Wang et al 2005) and hence using a breakup and coalescence model by different authors with different underlying principles (and fitting parameters) seems erroneous to me. However, considering literature, Wang's or Lehr's model is likely more accurate - I hope future versions will include these for coalescence, too (or if someone has a UDF implementation, if you could share it...)

With models selected, set boundary conditions. you will need to supply at least classes/moments at all inlets, and probably also at outlets for possible backflow. It's also good to use patch to fix an initial bubble size in the entire domain (I typically just put everything in one class there, between 2 and 5 mm depending on expected outcome). Then run. Higher order schemes may be problematic, start with first order and see if you can go better afterwards.

Good luck!

We use ANSYS-CFX.

Before spending a lot of effort in trying to combine CFD and PBM, consider the following:

1) Use one average gas bubble diameter in the two-phase model. That hangs together with trying to find out how much you really gain in descriptive / predictive power by considering bubble size distributions, compared to a situation where you do not consider that size distribution

2) Do you have supporting data? There is little or no point in simulating a gas bubble size distribution by combining CFD and PBM if the size distribution cannot be validated experimentally.

3) Skip the CFD model, and combine the PBM with a compartment model instead. Simulations will run much faster. If you are satisfied with the results, you can always move on to CFD+PBM afterwards.

Hi Cees,

Thank you for the reply. Yes I first tried the single phase (water) and it is running well and also converging. Then I used the water/air as two phases and it was running, but the contours were not up to the mark as they should have been. Can I get some guidance from you so that I can run the simulations successfully for two phase with CFD-PBM model. Let's keep in touch.

Thank you!

Hi Krist,

Thank you for the reply. I am using ANSYS-FLUENT. Yes I am first planning to use a single bubble size in the two phase model. I don't have any experimental data supporting the bubble size distribution. Is it necessary to have the experimental data, because it is not so easy to get the experimental data. Can you elaborate on the compartment model as I have never used it so that I can also make use of it. Please reply.

Thank you!

Well, if you don't know the bubble size it will be difficult to set a single bubble size too, and and you cannot check if the outcome of your simulation in terms of BSD is correct. Besides, if your practical BSD is very narrow, there might not be a point in using a BSD; a single bubble size is sufficient. So it is strongly preferred to have experimental backing.

You may be able to comment on your results based on some other parameters. A colleague of mine ran simulations for a large fermentor with 3mm and 5mm bubbles based on sparger configuration without success; the gas holdup and flow profile were off (hold-up was known, and operating regime). With a PBM the mean bubble size was predicted to be 8-9mm in the bulk of the domain, and hold-up results, flow-pattern were in good agreement with industry data, kla and mixing time were reasonable (using 8mm single bubble size yielded similar results, so a BSD was not strictly necesarry there). However, since the bubble size is unknown, it could does not automatically mean this large bubble size was correct - it could also be the presence of surfactants and such altered drag, for example.

We later used this approach in a mixing study; we were not interested in the BSD there, just mixing behavior (and we could verify that) but it would be difficult to translate said simulation setup to a different situation. If you want to know whether your setup gives meaningful results in terms of bubble size, you are going to need the experimental data.

Hi Cees,

Thank you for the reply. I can use a single bubble size using the Moo-Young correlation and I found one research article where they have used this correlation for the simulation without the PBM model. I am sending you the same article here as attachment. In this paper, Can you please help to explain how they have selected the bubble classes. Please reply.

Thank you!

Hi Sohail

We did use the PBM model in this simulation.in 2008 and it was before that Fluent integrate it. So reread the article every thing is well explained in there