One of the question I have seen frequently is how to set velocity inlet for individual phases wen using VOF multiphase model in fluent.

I do agree that Fluent is a very good software with lot much flexibility but still it has certain descripensies which need to be addressed sensibly. First, its like a black box and u need to put some thinking about ur possible flow looks like and then depending on it generate a mesh and simulate ur model.Our understanding of physics is a must to get reasonalbe results in least time.

Here is a question, which I like to state a possible solutions depending on my experience using fluent VOF model.

QUESTION:

How to set volume fraction in two phase flow

Dear Rizwan: Thanks to the replay. Yes I was defined the air as primary phase and water as secondary. If both of the phases enter from the same inlet but with different velocities can you tell me how can I did that?

Thanks a lot

MY REPLY:

In fluent, VOF doesnt allow us to specify velocities of individual phases. we can only specify velocity of hte mixture. I would suggest two approches to resolve this issue.

1. modify ur geometry to make two inlets and a common outlet. on common understanding in real time physics, what we have is air occupies the upper portion of the pipe. so for the top inlet specify velocity u desire for mixture only, but the secondry phase vof for top portion be 0. the lower inlet, will have vof of secondary as 0.25 and the remaining will be primary phase. here too, we speicfy velocity of mixuture only. but u will drastically reduce the chances of reducing the computer simulation tym as well as gettign some realistic results.

2. write a udf using DEFINE_PROFILE for a multiphase problem using all the looping macros specific to multiphase flows and set velocities fro individual phases. this is not tough but a very realsitic one to ur case.

I would also like to take the liberty of posting the same solution along with ur querry on CFD online, as I came accross this question quite a bit of time.

Hope this helps Best Regards All the best Rizwan.

Dear Rizwan: I want to command about the first point of your answer. How can I modify the geometry for two inlets? Did you mean I did that through Gambit? Can you explain for me this point in more details?

Regards

K. Baker

Hi Razwan: I have horizontal pipe. I not think the height of inlet can be estimated as (0.25*pipe diameter) & (0.75*pipe diameter) for both water and air respectively even for horizontal pipe and let the others give us their opinion about this if there is anybody can answer? The water cut as you know = Superficial Velocity for water divided by The velocity of mixture (which is the sum of the two velocities for air & water). So I think the water cut the same as the volume fraction at inlet and not a ratio for diameter of pipe? What did you say I need to know your commentary about this?

Thanks K. Baker

Well I think u got me wrong. what i meant by saying about conditions 0.75*dia and 0.25*dia at inlet is to give some realistic boundary condtions and then allow fluent to calculate for the rest of domain the hold up etc of individual phases.

As you might be aware that the inlet condition is a sliced part of c/s of the pipe. so giving an inlet condition in the above speicified way will suffice ur need of setting velocity for individual phases. I like to mention tht even though u will specify velocity of mixture wen using vof model in fluent, due to defining of phase fractions at top and bottom inlet conditions as 0 and 1 for secondary phase, u r in a way specifying velocity of individual phase. this will have a secondary advantage of reduced the time to simulate at the same time assuming and assigning a realistic boundary condtion.

Regards Rizwan.

In any of the methods the time will be less , in your method of making separate inlets for each phase or in mine by considering one inlet with a mixture velocity. Did you think the two methods give the same results?

K.Baker

if u r solvign for steady state stratified horizontal pipe flow, the results should be same. now it depends on steady state or unsteady state u r solving, in first place. it the pipe inclination is non zero with horizontal, then surely the holdup at inlet and outlet is not the same.

Regards Rizwan.

Did you mean that holdup not change with time and axial distance if the pipe inclination be zero? I have a paper in this case but the holdup changes in it with both of time and axial distance?

K.Baker

well if its unsteady state, and if u prepare ur geometry and specify the boundary conditions in the way i said, there will be very small change in hold up till the flow adjsuts itself with change in magnitude in the enitre domain. u will not see a real mixing of fluind in individual cells.

but with a single inlet, wat happens in a numerical solution is, based on the inlet conditions as 0.25 secondary phase, this much amount of secondary phase is initialized in each cell irrespective of where it exists. from then it goes on to solve and separate the fluid, with the denser fluid setlling in the bottom.

I best advice that u giv a try to both of them and see wat actually happens in either case then u will be better undrstanding how vof is solved in fluent.

I have been using VOF for over a year for my thesis problem which is quite complicated involving dynamics of solid particles, multiphase as well as unsteady, this has been my experience.

Regards Rizwan

I want to thank you for your valuable answer. Did you have idea about using the open channel flow boundary which available in the VOF model. I thought this boundary can be used only with one inlet? Can you tell me what the total height and the button level in this boundary mean?

Khalid

No I dint use open channel flow. My study is specific to stratified flow only.

Regards Razwan

Its also used with stratifed flow.

K.Baker

Its

I am supposed to model flow through an air lift pump using fluent,Slug flow through a vertical pipe that gives me maximum efficiency (Mw/Ma).I tried using VOF method but the solution diverges and it gives me an error.Air is being injected horizontally small distance from the bottom of the pipe and water is being sucked from bottom. Would you please help me how to handel this problem such as b/cs or how to model Taylor bubble rising through a vertical pipe. Thanks

[monty_p20]

Hello Rizwan, Baker..

Can you help me also about water droplet simulation through pipe(channel) using
VOF model in Fluent.

Thanks

[lixuan1126]

Originally Posted by Abe
;140491

I am supposed to model flow through an air lift pump using fluent,Slug flow through a vertical pipe that gives me maximum efficiency (Mw/Ma).I tried using VOF method but the solution diverges and it gives me an error.Air is being injected horizontally small distance from the bottom of the pipe and water is being sucked from bottom. Would you please help me how to handel this problem such as b/cs or how to model Taylor bubble rising through a vertical pipe. Thanks

Dear Abe, I'm also working on an airlift pump which is same as your case. could you tell me how to do this. I'm trying two inlets, one is pressure inlet for the bottom water, and the other one is velocity inlet for the air from side. However, there was only one Taylor bubble occurred. Other bubbles broke up and stick tightly on the pipe wall. I have no idea about this. My adviser said the surface tension I set might be wrong (I used 0.072n/m). BTW, water was set as the primary phase. Is is related to this? Looking forward to your reply.

[rahul8dev]

How to define CO2 gas as a first inlet and CO2 liquid as second inlet Using VOF method??
Please Help me to solve this problem.