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.

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!

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.

- 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):

- 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.

- 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.

- 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.

- 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.

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.