[miles_davis]

Hi

I am simulating the flow in a water box equipped with a nozzle in the bottom.
The nozzle injects a mix of air and water (alpha = 0.1)
After some reading on this kind of flow on this forum I have chosen the twophaseeuler solver.
To initialize the flow I have taken the velocity distribution for a case with only water.
I have reproduced the settings of the bubble column tuto. Except for the drag force.

A t=0, I start to inject some air.

What i do not understand is that after a few iteration I get a full air velocity field even in region in which the air is not present
I have the impression that this strange behavior is due to the fact that OF calculates my air velocity by scaling the water velocity.
Why is this happenning?

If any body has some advice I'd be glad.

Another question concerns the pressure field. Since the box is filled with water the pressure changes with altitude.
So I don't want to impose pressure at the outlet of the domain.
What alternative type could I put?
If I put an inletoutlet velocity condition what is the corresponding condition I should use for pressure?

Thanks a lot

The picture illustrating my case are given.

[grjmell]

You've fixed the pressure at the top, so zeroGradient on your outlet should work...

[miles_davis]

Thanks for your answer.
I put a zero gradient at the outlet but due to the recirculation I have some flow in and out the exit surface, So I may try a inletoutlet BC.

Do you have any guess why Ua is indexed on Ub even when specie A (i.e. air) is not present? In should be zero in such case.

Thanks again.

[miles_davis]

Hi
I have solved my pressure distribution problèms.
What I do not get it's why and how a velocity of a phase that is not present in a fluid domain (i.e. vol fraction alpha=0.0) can be non equal to zero????!!!!
I am using twophaseeulerfoam.
I have reproduced the tuto of the bublle column and i have found the same issue when velocity is set to zero at the beginning.
Please has anyone any guess where it might come from?

regards,

[alberto]

Hi Miles,

Originally Posted by miles_davis

What i do not understand is that after a few iteration I get a full air velocity field even in region in which the air is not present
I have the impression that this strange behavior is due to the fact that OF calculates my air velocity by scaling the water velocity.
Why is this happenning?

This is due to how the momentum equation has been written. OpenFOAM uses the phase-intensive form of the momentum equation, meaning that the original phase momentum equation is manipulated so that it can be divided by the phase fraction.

This is a quite common approach in many codes for nuclear safety applications and it was also adopted by Oliveira and Issa in one of their papers.

The phase-intensive momentum equation has the (correct) property that it makes the velocity tend to the particle terminal velocity if interaction terms are removed.

In other words, seeing a non-zero velocity where alpha is zero, is expected. However this should not lead to problems since all the terms depend on alpha.

Best,
Alberto

[miles_davis]

Dear all,


Thanks a lot for your answers.
I have another question.
I try to reproduce a two phase flow simulation made with Fluent.
It is the same case as described above except the fact that I do not simulate the air volume above the free surface of water.
I have concerns about the BC to define for the free surface and the outlet.
For the free surface for principal phase (i.e. water, phaseB) I use the slip BC on Ub.
I am confused for the air (phase a). The air can flow out of the domain at the free surface. Therefore witch BC do you think would be suitable for velocity Ua and alpha?

I have the same concern for the outlet.
I enclose to my post a picture of my test case and the BC I want to define.
Thanks a lot for your help and advices.

Regards,

[arjun]

Originally Posted by miles_davis

Dear all,


Thanks a lot for your answers.
I have another question.
I try to reproduce a two phase flow simulation made with Fluent.
It is the same case as described above except the fact that I do not simulate the air volume above the free surface of water.
I have concerns about the BC to define for the free surface and the outlet.
For the free surface for principal phase (i.e. water, phaseB) I use the slip BC on Ub.
I am confused for the air (phase a). The air can flow out of the domain at the free surface. Therefore witch BC do you think would be suitable for velocity Ua and alpha?

I have the same concern for the outlet.
I enclose to my post a picture of my test case and the BC I want to define.
Thanks a lot for your help and advices.

Regards,

here are few questions:

1# Alpha = 0.1 , means that 0.1 x Water + 0.9 x Air? Am I right.

2# Wouldn't it be better to define a new fluid with properties derived from alpha x Water + (1-Alpha) * Air , should be called Steam and solve for this fluid. So main phase would be steam and secondary phase would be water. At inlet Alpha = 1 then.

Am I wrong about it, are there problems in this approach that would give wrong results? Please correct me.

3# what are the geometric dimensions of box you presented as domain. This I am asking because currently I am trying to write VOF code myself and if I get time would like to run your case myself. (If possible, just for pleasure and fun).

[miles_davis]

Hi,

sorry for the delay of answer

Originally Posted by arjun

here are few questions:

1# Alpha = 0.1 , means that 0.1 x Water + 0.9 x Air? Am I right.

sorry I was'nt clear enough:
alpha is the vol fraction of air
so in fact it's the opposite:
0.9 watter
0.1 air

Originally Posted by arjun

2# Wouldn't it be better to define a new fluid with properties derived from alpha x Water + (1-Alpha) * Air , should be called Steam and solve for this fluid. So main phase would be steam and secondary phase would be water. At inlet Alpha = 1 then.


Am I wrong about it, are there problems in this approach that would give wrong results? Please correct me.

No
I can't do that.
It's a filtration process.
So I want to see how air and water separate.
So I don't want to define a mixture of air+water.

Originally Posted by arjun

3# what are the geometric dimensions of box you presented as domain. This I am asking because currently I am trying to write VOF code myself and if I get time would like to run your case myself. (If possible, just for pleasure and fun).

It is a square box of 2mx2m
inlet: 0.5m
outlet: 0.25m

Regards,

Miles

[arjun]

Originally Posted by miles_davis

Hi,


It is a square box of 2mx2m
inlet: 0.5m
outlet: 0.25m

Regards,

Miles

I was able to run your case. So far it is 'Colourful Fluid Dynamics', it does show me some results. Look alright to me. (off course not usable).

There are few things:
1. I did not know the nozzle design so i just used slit of 10mm as inlet. My guess is that inlet is smaller than this in diameter.
2. About the free surface at top, I used outflow condition. That is in this case flow can go out and some of it can come in.

Question: Can flow really come in and go out of it. OR it is closed??

3. I extended the outlet part and fixed it to a pressure boundary condition.

Anyway i do not have problems, SO FAR, solver runs fine (at least for last 10 minutes that i tried ).


PS: I did not run it fully, but here is where i stopped it.

[miles_davis]

Hi
Great simulations.
Is it made with your own code? What method it is? VOF?

The problem is the BC at the top of the domain.
Since it is air in a water box, the water can't escape from the upper surface.
That's why I need to fix a different BC for water phase and air phase!!!
And since I need two study diameter sensibility, I am stuck with twophaseeulerfoam model.

Another question:
what did you put as a BC for the outlet?
p=0?
Why did you add this long duct at the outlet?


regards,

P.S.: does anyone know what is pressure in OF2.0.1?
I have read that in previous version of the code it was in fact Pstatic-rho*g*h, than in antother version it was just Pstatic. What is the actual statement for OF 2.0.1?

[arjun]

Originally Posted by miles_davis

Hi
Great simulations.
Is it made with your own code? What method it is? VOF?

Yaa, I am trying to learn and implement VOF methods. I am finally able to validate the explicit version.
I am following this paper:

http://webfea.fea.aub.edu.lb/cfd/pdf...S-Complete.pdf

The code is same as discribed in this paper with a minor change from my side, instead of SUPERBEE , I am using Bounded Downwind of HRIC scheme.

Results are impressive so far, but I would now try to make it implicit.

Originally Posted by miles_davis

The problem is the BC at the top of the domain.
Since it is air in a water box, the water can't escape from the upper surface.
That's why I need to fix a different BC for water phase and air phase!!!

You see, since volume fraction only convects by advection equation, it could only go through top if velocity across it is finite. But if velocity across it is finite water can escape and enter from top.
I think partial blocking of water , though possible by modifying code, is not suggested.

Originally Posted by miles_davis

And since I need two study diameter sensibility, I am stuck with twophaseeulerfoam model.

Another question:
what did you put as a BC for the outlet?
p=0?
Why did you add this long duct at the outlet?

the outlet is at the moment pressure outlet, this is why I extended it. (other reason to extend it was possible recirculation of flow at exit you had that might create problems with solver).


BUT, I could switch to outflow conditions instead of pressure outlet, where pressure at only 1 point is fixed (not at whole outlet).


Usually in the solver when you have outflow conditions solver tries to balance the mass flux and make it equal to flow coming in through inlets.

For running your case I had to switch that thing off.

So thanks, now I can provide user an option to switch forcing of mass balance at outflow. Before your case it did not occur to me.


PS:

I am solving for air and water is my secondary phase. This means VOF equations are solved for air and water C = 1 - Air_C

[miles_davis]

Hi ,

I have kept on trying to simulate air injection with the Twophaseeulerfoam.
After having performed a transient simulation of the water injection, I added the air.
The air bublles diameter is 150µm.
I take into account drag with a shcillerneuman model (I have reproduced the bubble column tutorial for drag interaction but I hope the reading of Rush thesis will give me a better rule of choice for bubble drag).
Lift and virtual mass. Are on as well.
I get a rising air flow (see picture)

What I do not understand is why the velocity of the buble remain strictly aligned on the water velocity.
it seems that drag effects are very high and so bubbles stay in close contact with the air flow.
I was expecting buoyancy effect to help bubble to rise faster than the water flow!

I am currently reading
Numerical aspects of an algorithm for the Eulerian simulation
of two-phase flows
Paulo J. Oliveira
Raad I. Issa
and the thesis from Rush.

It seems that buoyancy effects are indeed taken into acount.
So I do not understand why I can't reproduce these effects with the model.
Maybe I misunderstood something in the model.

Thanks for your help.


Regards,

Miles

[miles_davis]

Hi,

I have made a test: a simple volume of air in the domain at the beginning of the calculation.
It appears that the air is rising in the water due to buoyancy effect.
So this is not the problem in my simulation.

I have run another tests and in every case for d<500µm, the velocity field for watter and air are exactly the same. As if the drag force of water on air bubbles tends to infinity.
I have checked and read the solver, I do not see anything strange in its formulation.

Has anyone ever encountered such problems?

Thanks for your help.


Regards,

[alberto]

What is the injection velocity of the air in the real system you are simulating? Is it consistent with your setup?

If the air is injected at a high enough velocity, it will clearly create a sort of jet.

Best,

[miles_davis]

Hi,

The air enters at the same velocity as water: 0.2 m/s.
And it does create a jet.
I am ok with that.
My concern is on the fact that at the free surface of water, I was expecting the bubble of 150µm to continue rising and escape!
But they reach the surface and slip on the free surface as the water.
Besides the air velocity is strictly alined on water velocity.
I have to check Stokes number but it seems wired.

Regards,

[cyw]

I want to simulate bubble injection from a nozzle in the bottom. Could you please tell me how did you build the geometry of the nozzle? Thanks for your help!

Originally Posted by miles_davis

Hi ,

I have kept on trying to simulate air injection with the Twophaseeulerfoam.
After having performed a transient simulation of the water injection, I added the air.
The air bublles diameter is 150µm.
I take into account drag with a shcillerneuman model (I have reproduced the bubble column tutorial for drag interaction but I hope the reading of Rush thesis will give me a better rule of choice for bubble drag).
Lift and virtual mass. Are on as well.
I get a rising air flow (see picture)

What I do not understand is why the velocity of the buble remain strictly aligned on the water velocity.
it seems that drag effects are very high and so bubbles stay in close contact with the air flow.
I was expecting buoyancy effect to help bubble to rise faster than the water flow!

I am currently reading
Numerical aspects of an algorithm for the Eulerian simulation
of two-phase flows
Paulo J. Oliveira
Raad I. Issa
and the thesis from Rush.

It seems that buoyancy effects are indeed taken into acount.
So I do not understand why I can't reproduce these effects with the model.
Maybe I misunderstood something in the model.

Thanks for your help.


Regards,

Miles