Dear All,

Does anyone have any experience in simulating slug flow using Fluent's VOF model????

Any help will be appreciated.

Thanks in advance

Hello Paul,

Can you be more specific? Is it horizontal or vertical slug flow? Which fluids? I have experience in the simulation of horizontal two-phase flows, making use of the VOF model. If you can be more specific, maybe I will be able to help you.

Greetz, Sandra

I am simulating slug flow through a horizontal mini channel, I have adpoted the VOF model with a constant surface tension. I have also assumed the flow to be laminar

For BC: I have specified a constant velocity inlet of 4.2e-3, an outflow and non-slip wall condition.

For IC: I have patch a arbituary sized gas bubbles cylindrical in shape in the channel (volume fraction 1)

The square channel of size 2 x 2 X 50 mm grid size of 26 X 26 X 635

I have tried to reduce the under-relaxation factors but was unable to get satisfactory results. Do you have any suggestions to resolve the problem? Did I miss out any other parameters/conditions required?

Sincerely appreciate your kind assistance. Thanks in advance.

Hi Paul,

When I want to perform a two-phase flow calculation, I always start with the converged solution of the flow of one the phases. This increases the stability of the two-phase flow calculation.

Maybe you can try this first. However, if you still have problems, let me know.

Greetz, Sandra

Dear Sandra,

Thanks for the advice. However, i am still having problems with the simulation. I recieve this error message :

"Too many (1859) VOF sub-timesteps. The velocity field is probably diverging. Please check the solution, and reduce the time-step if necessary"

while iteration.

What does this error message means?

Hi Paul,

This means that the time step that you have defined for the unsteady simulation is too large. I always use 0.001s, normally this time step should be small enough to avoid divergence. I hope this can solve the problem.

Greetz, Sandra

Dear Sandra,

Can i check with you on what is the initial and boundary conditions that you have used? Also did you include any other factors like surface tension and contact angle for your 2 phase simulation?

Thanks alot for your help

Best Regards

Dear Paul,

I did include a constant surface tension for the simulations. I did not define any contact angle. I always used the geometric reconstruction scheme for the reconstruction of the interface.

Concerning your divergence problem, I don't see a solution right away. For me, reducing the time step was always the solution. Maybe you can increase the number of VOF iterations in each time step and you can also decrease the underrelaxation factors for the calculation of the velocities. I hope this will work.

Greetz, Sandra

Dear Sandra,

Sorry can i check with you how do i change the number of VOF iteration for every time step?

And also how does Fluent takes into account the capiliary forces?

Thanks for your advice. I will try on it.

Best Regards

Dear Sandra,

Sorry to bother you again.

I have tried to reduce the time step from 0.001s to 0.00025s but i will still get the same error msg when the iteration hits time 0.002s.

Do you have any advice on this?

Thanks in advance for your help

Best Regards

Usually when you model this kind of flow with hihly curved interfaces, you need a very very small time step.... The interface should not move by a distance less than the size of one grid size.

Another problem could be also the curvature of the interfaces versus the grid size. The 1/curvature at any point should be smaller than your grid size. In practice, this means that a drop should be much bigger than your grid size.

To get bigger 1/curvature, increase slowly the surface tension by a factor of 10-1000, and start again your calculation. If your calculation is better....then this was the reason.

By the way what VOF method are you using....

Dear Kharicha,

Thanks for your kind advice.

I will be trying your suggestion.

I am using the geometric reconstruction scheme to reconstruct the interface.

Best Regards.

If you have a very long interface(many bubbles), the geometric reconstruction will be to heavy for you.

I suggest to you to use more stable method as implicit....

Dear Kharicha,

I am simulating the flow of a slug bubble through a square channel. So there is only one bubble in the domain.

I have tried increasing the surface tension and it seems that the calculation seems to get worse. so i was wondering if i should reduce the mesh size.

I am currently using a mesh size of 0.05 x 0.05 mm.

Thanks for your kind help

Best Regards

You can increase the value of surface tension only if your interface is smooth.... to get a smooth interface, initialize your system, ...i.e patch your bubble domain.

Now you can see that the interface is irregular, following your mesh... Switch to "implicit" version of VOF, do several time iterations with your surface tension value.

You will get a well shaped bubble.

save the results..data

then switch to georecontructor version of VOF. If it is converging, then keep it like that...

if no, then come back to "implicit", and increase slowly the surface tension, then again come back to "georeconstructor"....

If it doesn't work, I will need more details...

Dear Kharicha,

I have tried implicit method but the iteration was unable to converge.

Thanks in advance for your kind help

Best Regards

Dear Kharicha,

i have reduced the time step for the iteration to 1 e-5s and there is no problem of divergence.

However the solution the i am getting is not as expected. That is the shape of the resulting bubble is not as expected.

Is there any advice u can give me?

Thanks alot for your kind advice.

Best Regards

The solution you can get is highly dependant on the curvature definition of the surface of your bubble. So did you reach grid independant results ?

You can also use adaptive mesh refinement technique to increase the number of cells only at the interface....

[akchetty]

Hello,

I have been trying to perform vertical air-glycerol slug flow simulations in Fluent using VOF and was thinking if you can help or give an advice regarding the issue I am facing right now. The terminal velocity I am getting for a rising taylor bubble in stagnant glycerol solution is only half of what it is supposed to be according to literature and other CFD results in the paper (Numerical Study of Hydrodynamic Characteristics of Gas–Liquid Slug Flow in Vertical Pipes). I tried following the methodology people have used in the literature, the one of solving the two-phase set up in a frame moving with the Taylor bubble. So I have the two walls moving downwards (2-D domain ) along with the liquid (top- velocity inlet and bottom - outflow) at terminal velocity of the taylor bubble. Unless I use a velocity value almost half of the correct value from literature, my Taylor bubble either moves up or down the domain. I tried using stationary domain but still I am having the same problem of half the terminal velocity. I am using pipe diameters of 19-22 mm and mesh sizes of 1-0.5 mm and initially start with a film thickness calculated from empirical correlations and start with a bubble length of 3.5 times the bubble diameter. My solution converges, but terminal velocities are off by half. Any idea or suggestion regarding where I may be doing a mistake ? Looking forward to your reply. Thank you.