[hilde]

Dear all,
I am trying to simulate a small reactor in CFX 15.0 using a multiphase (air at 25 deg + water at 25 deg), inhomogeneous, free surface steady state model. I am using a homogenous turbulence model and a closes system.

The reactor is approximately 1 cm in diameter and has a rotating propeller element inside of it. There are no baffles on the walls so I am using a rotating domain for the entire geometry with counter-rotating moving walls on the reactors outer surfaces. I have cut the geometry in two and am using rotational periodicity between the two cut-surfaces.

For the rotational speeds I am simulating, the Reynolds number is ca 400-2000 for the water and lower than that for the air phase.

I have created 3 different tetra-dominated meshes with ca 30 000, 80 000 and 160 000 elements in each.

Once simulating, I am however facing the following situation:

• Once using the laminar model, it converges very fine for the lower Reynolds numbers for the coarsest mesh
  
• Once using the SST turbulence model, it also converges very fine for the lower Reynolds numbers for the coarsest mesh
  
• I have not been able to make neither the laminar model nor the SST model to work for the second finest mesh.
  
• Once using the k-epsilon turbulence model, it converges well for all meshes and for all Reynolds numbers simulated.

With nice convergence, I mean that the residuals are more or less constantly decreasing over time and that my monitoring points (velocity, torque and epsilon) reaches steady values.

So, the trouble arises for the finer meshes where no convergence behaviour is reached. In some of the cases, the residuals and monitoring points are showing just a chaotic behaviour and with other settings, they are both oscillating in a periodic way.

These periodic oscillation are, as I have understood it from various posts, a clear sign that my systems is actually transient and that I then should do a transient simulation.

I have tried with transient simulations starting with down to a tiny (?) initial time step (around 10e-7 s) and adaptive time step but have given up on them due to lack of positive outcomes.

I have also a very hard time understanding and visualizing how my system could be transient since it is a closed one and the rotor element in the middle is moving with a constant rotational speed, and since the simulation worked out fine for the k-epsilon model and for some of the laminar and SST ones.

For the laminar model, I somehow feel that the transient behaviour could arise since the system is not fully laminar and it is trying to perform some “turbulence behaviour” with the finer meshes. However, this explanation does not explain why the same problem arises with the SST model?

I am also not really happy about using the k-epsilon model since as I have understand it is best for fully turbulent, non-rotational, free stream flow which is basically everything my system is not.

In order to sort this out for the finer meshes and the laminar and SST case I have tried various things such as

• Using the coupled solver
• Using a hexa-dominant mesh
• Using an homogenous model for the velocity
• Initial values created with the upwind scheme
• Creating a small opening in the top of the domain in order to not have a closed system anymore
• Various different physical time steps and also automatic time

None of this has solved the overall problem, even if the coupled solver for example made it somewhat better. However, I have not found an overall working solution an am starting to run out of resources to work this out on a “try-it-all” basis.

So, I would very much appreciate any kind of input here on what could be wrong and if anyone of you have any idea where it is good to spend time on searching for solutions. (For example spending time into making a structured (blocking) mesh of the entire rather complex geometry? Or trying a transient simulation with even smaller time steps? Or removing the rotational periodicity and instead simulate the entire reactor? Or something completely new that has not crossed my mind?).

Please also let me know if there is anything unclear in what I am up to

Thank you in advance

Hilde

[ghorrocks]

Interesting question. Rather than answer your questions we should first confirm the basic models selected are appropriate:

1) Are you sure this thing is turbulent? The Re you suggest is laminar to low turbulent, but the turbulence threshold varies for different configurations. Also, multiphase flows can suppress turbulence transitions to higher Re numbers (due to the damping of the interphase drag). Unless you can show this flow really is turbulent then I would run it laminar.

2) Why are you using inhomogeneous simulation? Do you expect a free surface combined with a froth or bubbly region? Can you describe when the flow inside the chamber should look like?

3) You mention this is a reactor vessel. Is the reaction important at all for the simulation?

[hilde]

Thank you for the reply and sure it is a good idea to sort this out first!


a) I am not sure if it is actually turbulent or not, and am not really sure how to decide that more than looking at the Reynolds numbers? I have calculated the impeller Reynolds number according to the formula for stirred vessels = Turn per sec*Stirrer Diameter^2*Density/Viscosity. According to [1, page 205] it is dependent on the geometry of the tank and impeller if a certain Reynolds number gives a turbulent flow or not for a stirred liquid. It is said to be laminar for Re<10, turbulent for Re>10 000 and transient all in between. So it should, as you say, be either laminar or low turbulent.

However, the laminar model and the SST model only seem to work for 200, 400 and 600 rpms and as stated before and only for the coarsest mesh, so I am not sure if it is not working for 800 and 1000 rpm since it is too far into the transient regime to manage that or because there is something else wrong with the model.

Have anyone of you any recommendation on which turbulence model that should be best used in this transient regime?

The reasons why I used the k-epsilon and the SST in the first place is that they seem to be most commonly used in my field, which is simulating oxygen transfer in bioreactors. The oxygen transfer capabilities of different configurations are then often related to the turbulence eddy dissipation in the reactors. An example of this is [2] where the SST model has been used for two phase free surface flows, but with the slightly higher Reynolds numbers 2356-6281. But, if my system is not turbulent it would not make any sense to use turbulence model to model it. But on the other hand, if it is early transient and the laminar model does not work it does not leave me with any choice it feels like?


b) I have been using an inhomogeneous model since that is what I interpreted have been used in [2] according to the authors PhD thesis [3].

I also tried using the homogenous model, but then fractions of air ended up stuck in my liquid with no chance of escaping it. With the inhomogeneous model this did not happen and I got two nicely separated continuous phases. However once thinking about it, it feels like the homogenous model should work if I just could avoid to get those fractions of air to get stuck under the surface during the star-up of the simulation?

About the appearance of my flow, I have all the time assumed that there should be no bubbles in the liquid domain and am therefore using two continuous phases. But I am unfortunately not sure if the mixing blades are whipping in some air into the water phase in reality.

For illustration purposes, I have now attached a picture of my reactor and the 0.5 volume fraction isosurface for 1000 rpm (Re= 1900) using the inhomogeneous model so you all can see a bit how it looks like.


c) I will not implement any simulated reaction in my reaction. I will however simulate mixing in it by simulating the spread of an additional variable. This has already been done for the k-epsilon model and gave decent results compared to experimental mixing experiments.

I am also interested in the turbulence eddy dissipation in the reactor since that seems to be what “everyone else” is using for simulating oxygen transfer in similar systems. But this is again all dependent on if I can allow myself to use a turbulence model without feeling bad about the system not really being turbulent.

But no, no reactions more than that and definitely not any phase changes.



I am sorry if this got a bit long again, but I hope it is somewhat the answers you were looking for and that it made my problems more clear.

And again, I do very much appreciate all help and attention this problem can possibly get


References for the interested:

[1] https://books.google.dk/books?id=Z-N...207.24&f=false

[2 ]Brüning, S., & Weuster-Botz, D. (2014). CFD analysis of interphase mass transfer and energy dissipation in a milliliter-scale stirred-tank reactor for filamentous microorganisms. Chemical Engineering Research and Design, 92(2), 240–248. doi:10.1016/j.cherd.2013.07.024

[3] Brüning, S. (2012). Technische Universität München Strömungssimulation als Werkzeug zur Bioreaktorcharakterisierung

[ghorrocks]

a) If the low is laminar and low/transitional turbulent then I would probably use a laminar flow model for all models. The issues you say about convergence are a numerical stability issue and should be addressed by other means.

b) The choice of physical model (inhomogeneous/homogeneous) should be made only based on what the flow condition is. So if the flow has two distinct phases with no bubbles then it sounds like the homogeneous model with a free surface model is the one you want.

c) OK, good, that simplifies things.

So I would recommend considering a laminar model with homogeneous free surface model. You probably will have numerical stability issues with it, remember the model important issue is mesh quality so a high quality hex mesh will help if you can do it.

[hilde]

Thank you very much again! I have currently re-built the mesh to a hex-core one with more and finer prism layers and am running the homogeneous, free surface simulations now. Will see how it develops, but of course hopefully in a good way!

[ghorrocks]

As this simulation is laminar to low turbulent it means your boundary layers are likely to be very thick, or probably not a coherent boundary layer at all. So rather than using a hex core with inflation mesh I would suggest a full hex mesh, with only a little refinement at the walls. Your geometry appears simple enough that a pure hex mesh should be possible.

Have a look at your results so far and see if you have much of a thin boundary layer. If you do not then consider my suggestion of a full hex mesh.