Using Fluent

The mesh

The first thing we have to do here, is to justify the reason why we have chosen a fixed mesh rather than an adaptative one.
One solution could have been to refine the mesh around the interface at each time step. Yet, after having tried this solution, it appeared to us that it was very very constraining to do such a thing with Fluent. As a matter of fact, the calculations are so long that even with a lot of will, we have aborted this attempt.
Further, to refine the mesh, Fluent require an unstructured mesh, what makes the calculations still longer!

From that moment, the only choice was to use a fixed mesh.
Concerning the number of cells, we have found that a good compromise between the time for one iteration and a sufficient number of cells in the bubble was to use a grid made of an estimated 10000 cells, that is to say 100 cells by 100 cells.

Another important point is that, when using the axisymmetric solver, you create a mesh only for the half of your domain, thus reducing drastically the number of cells you use, and consequently the time of calculation.

Be careful, Fluent prefers when your axis is the X one. So, make sure that you do not choose an axis that is vertical.
Considering the fact that our bubble will be centered in the column, we have also squeezed the mesh up near the middle, so as to have a good precision in the vicinity of the bubble, in an attempt to avoid useless heavy calculations at the limits of the domain.

At last, the mesh is different for each case, because it is impossible to use the same grid for both a bubble of 6 cm and one of 6 mm.
Nevertheless, here is how our mesh looks like.


- The mesh -


Before starting to iterate

To avoid surprises after o long and hard calculation, here is a quick check list of what you have to do to well configure Fluent when simulating to phase flows. For further details and pictures of the windows opened, or if you just want something nicer, please report to direction for use we have made.

Design a mesh that just represents half your domain because you will have to use the axisymmetric solver in Fluent

Define the inlet and the outlet as periodic conditions, so as to avoid reflexions that could give you bad results

Define the wall as a symmetric condition as well as the axis

In define-->boundary conditions, change the symmetry into an axis so that the solver understands why your are using the axisymmetric solver

In define-->model-->solver, click axisymmetric

In the define-->material panel, make sure that both water and air are present to be able to activate them in the next step

In define-->model-->multiphase, click Volume Of Fluid, then, you can click body forces (to enable gravity). Enable surface tension and choose the Geo reconstruct model, since it is recommended when you are especially interested in the shape of the interface.
If you want to be more precise, you can click solve VOF each iteration, but this may lengthen your calculations.
Of course, you have then to specify what is your phase one (the one that occupy most of the place): Water, and the phase two (dispersed): air

In define-->operating conditions specify that there is gravity, and do not forget that your axis have to be horizontal. So if, as it happened for us, you did a rotation of your domain, just specify that the gravity is equal to 9,81 along the x-axis.
Put the operating pressure to 100000 as well

In solve-->control-->solution, you have to choose the body force weighted scheme for the pressure discretization and the PISO scheme for the pressure-velocity coupling discretization.
Put the under relaxation parameters to one. If your calculations converge well (in few iterations), you can decrease some of them to something between 1 and 0,5.

To define a zone were you will put air, open the menu adapt-->region. Then you choose your geometrical form. A  sphere for us. You can then precise the x-center, y-center, and  the radius.
Then click on mark.
Note that Fluent writes the number of cells that have been marked. An amount of some dozen of marked cells is quite good. Do not try to launch a calculation with a bubble made of ten cells, because you will not get precise results concerning the shape of the bubble.
If you want to refine your initial bubble, refer to the directions for use

Now, you can go in the solve-->initialize-->initialize and init from all zones (if you do not initialize, you will not be authorized to patch!). After that, go in the solve-->initialize-->patch and click sphere_r0 (the name of your marked zone), phase density, and put a 1 in the zone reserved for the value. This will make Fluent consider that there is a density of air equal to one (that is to say only air), in the zone you have formerly marked.

Here it is, now you can iterate. Remember that the time step size have to be very small (10-5 for instance).
To generate a self-save calculation ...refer to direction for use!


Results

D=5mm

This what we had at the beginning of the calculation:
Now, we can draw what happens for two other time steps:

What strikes us is the deformation of the interface around the bubble. In fact, this is due to the diffusivity of the VOF model. You can improve this by clicking the solve VOF each iteration, but this is not always sufficient.
If we forget this default, we can observe that the shape of the bubble has not changed. This is not really astonishing, since the bubble is very small. And, as a matter of fact, we all feel that physically, such a bubble will not be deformed a lot.
Furthermore the Weber number (see the next chapter) is equal to We=6e-2. So if you remember the explanation for this number, you see that the interfacial tension is very strong.
The Bond number is equal to Bo=800.  But since it is the Weber number that determine the shape of the bubble, the Bond number do not give us any further detail.

It could be interesting to have a look at the vorticity and the velocity:

We can just notice that the maximum vorticity is located on the side of the bubble. Concerning the velocity, the mass added effect is clear.

Eventually, have a look at the end of the 1cm bubble section to have remarks on the recirculating zone clearly visible below.


D=1cm

a small animation
- a small animation of what you will observe for a bubble of 1 cm diameter -

What we see here is a spherical bubble which diameter is 1 cm.
At the beginning, the bubble makes a small oscillation (you can see it at the very beginning of the sequence). We can observe that the borders are moving around the middle horizontal axis of the bubble. This is very ensuring to get this with the calculation, because it appears to be what happens with a real bubble.

We can compare those results to the one we have found on the net (the IMFT web site):

IMFT reference !
- Results we were expecting -

We are quite close to what we were expecting. The simulation has just been stopped a little before the one found on the net.

If you want, we can have a look at what happens with the strain rate.

Strain rate!
- this is the strain rate at 1,2.10-1s -

You can observe that the point of maximum stress is, of course, located in front of the bubble, where the bubble penetrates in the water.

At last, we give an illustration of what happens with the dynamic pressure, that is to say the term in 1/2 x rho x V² that appears in the Bernoulli equations.

Pressure!
- velocity around the bubble -

Of course, the velocity is much higher in the back of the bubble, which is a rotational zone.

What could be very interesting to draw is the profile obtained with the velocity vectors, and the vorticity magnitude :
So, here they are :

We recognize the well-known shape called "en calamar", on the velocity vectors.
More seriously, we clearly see the vorticity location at the top of the bubble, as well as the Hill's Vertex inside the bubble. The velocity vectors reminds us that a recirculating zone is different than a maximum vorticity zone : we can see a circulating zone on the sides of the bubble, whereas the vorticity is almost negligible.
 


D=6cm


- here is a small animation of the results that we have obtained for this bubble -

The first thing we note is that what happens is definitively not pleasant. Yet, we have decided to plot those results considering the fact that such a calculation is very long, and that it teaches us something.

We have thought about it and we have thought that what happens here is probably due to the symmetric condition we have used at the bottom of our domain. In fact, if this condition is good for the walls, since it eradicates all interaction with the wall.

To explain the fact that the bubble explode into two other bubbles, we have thought that the motion of the bubble creates a motion of the water around. This motion of the water reflects at the bottom of our domain and then comes back in the back of the bubble thus breaking it. This is even easier, because the bubble is quite big here.

We will not study this case anymore, since we have not launched another simulation (lack of time). But here is a funny case where we have tried to see what happens with a square bubble.


Square bubble

We have decided to modelize something absolutely not physical: a square bubble. The dimensions are: 1,2 cm width and 0,6 cm high.
The procedure to initialize with this bubble is exactly the same than previously, except the fact that we adapt with a square.

Here is the initial bubble


- the initial square bubble -

What happens after a while?


- the square bubble at 1e-02 s 3e-02s and 1e-01 s -

First thing, we can see that the bubble is scotched against the bottom, thus explaining the fact that it has some difficulties to escape and conserve its shape.
After a while, we can hardly guess that it was not a bubble that was circular at the beginning, and it really looks like the one we have obtained upper with d=1cm.

Now, here are some quantities that may be interesting to see. The velocity magnitude for instance, the map of velocity with velocity vectors and the strain rate:

Those picture are to compare with the last one of the previous serie, that is to say, at time 1e-01s.
What we see is that the velocity is concentrated in the bubble and behind but never in front of it. Considering the second picture, you can see that the liquid is moving behind the bubble, and the motion is a rotation. There is a kind of recirculating flow behind the bubble. We can also notice the Hill's Vertex inside the bubble.
And last but not least, the strain rate shows that the effort are the greater just behind the bubble! Not really surprising.

Next