[PrzemekPL]

It's my first post on this forum so I would like to say Hello to everyone

I've been using OpenFOAM for a while and 'finally' (unfortunately I'm struggle with something. Let me experience myself as clear as I can.

My goal is to simulate slug flow in micro-reactors (T,Y-pipes and other odd shapes).
So far I was pretty successful using interFoam. Problems occurred once I've tried playing with Alpha Contact Angle (In order to get rounded bubbles in my system).

As usual I've started with simple test cases. Example you can see bellow. It's a liquid (properties similar to water) going through squared channel filled with water. Red color represents my liquid (alpha=1) and green color represents free surface.







I'm using OpenFOAM-1.6. My boundaries are:
inlet – constant velocity and pressure zeroGradient
outlet – constant pressure and velocity zeroGradient

I've setup static contact angle theta0 = 150, bellow piece of my 0/alpha1 file:

wall
{
type constantAlphaContactAngle;
theta0 150;
value uniform 0;
}

As you seen on the picture sort of bubble has been created so I assume that my settings are correct.


In next step I wanted to try with more complicated geometry which you can see on the picture below.




I left all the settings from the previous simulation. Only mesh was replaced (even patches names stay unchanged).
In this case my simulation doesn't converge and crash after few iterations.
Below you can see piece of logfile right before it crashes:

Courant Number mean: 0.00114123 max: 0.155363
deltaT = 8.19028e-06
Time = 0.00316112

MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = -0.00365136 Min(alpha1) = -6.40929 Max(alpha1) = 1
GAMG: Solving for p, Initial residual = 0.0788199, Final residual = 2.18146e-05, No Iterations 14
GAMG: Solving for p, Initial residual = 0.0228578, Final residual = 4.22779e-05, No Iterations 8
GAMG: Solving for p, Initial residual = 0.0019283, Final residual = 4.89251e-05, No Iterations 5
GAMG: Solving for p, Initial residual = 0.0010417, Final residual = 4.2426e-05, No Iterations 4
time step continuity errors : sum local = 6.32233e-08, global = -4.73033e-09, cumulative = -6.42826e-06
ExecutionTime = 154.77 s ClockTime = 161 s

Courant Number mean: 0.000549398 max: 0.0583325
deltaT = 9.5917e-06
Time = 0.00317071

MULES: Solving for alpha1
MULES: Solving for alpha1
Liquid phase volume fraction = -0.00366029 Min(alpha1) = -6.30349 Max(alpha1) = 1
GAMG: Solving for p, Initial residual = 0.00953035, Final residual = 2.05655e+141, No Iterations 1000

here it stops


So dear Foamers do you have any idea what's the reason of such a behave?

I just want to admit that it has probably nothing to do with mesh because with other settings everything is fine. By other settings I mean for example theta0 = 90deg. I think it has something to do with pressure because number of iterations on pressure jumped to 1000. But I have no clue why. This occurs only when I increase value of theta0 and only with this mesh. Previously (squared channel) I didn't experience any problems playing with contact angle.
I would appreciate any help.


Greetings!
Przemek

[sega]

Dear Przemek.

Welcome to the forum. Feel lucky you haven't met any problems yet.
Let me give you some thoughts I have about your case.

I assume you are prescribing alpha1 = 1 at the inlet?
My suggestion would be you try to initialize a small liquid volume at the inlet in addition to this boundary condition.
This means you will have some cells which are allready filled with liquid.
Maybe this will help the CSF-Modell to calculate the surface force and the pressure drop over the interface.

So far for a small brainstroming ...
Sebastian

[PrzemekPL]

Hello Sebastian,

Thank you for your quick answer.

Yes, I meant alpha1=1 at the inlet.

I need to tell you that I've already thought about initialization with some amount of liquid. In first case (picture bellow) simulation crashes immediately after start.




But have a look on the other example, it's pretty interesting. Initialization like before but with bigger amount of liquid.

At the first picture – time 0s..



Second picture - bubble shape has been created – negative alpha ( wtf???? )



Third picture (last results) – bubble became smaller.




You can't really see this on these picture but I've observed in ParaView that within each time interval (results saved every 0.01s) bubble was becoming smaller and smaller. I got impression like it was mowing back (sucking into the inlet). It was probably part of bubble forming, but I might be wrong. And again negative alpha, in the area of inlet corners.

Maybe this will contribute something to our brainstorming

Regards,
Przemek

[PrzemekPL]

In my further investigations I've initialized simulation by putting some amount of liquid far away from the inlet. I wanted to check if bubble can be formed from squared shaped volume.
Additionally I've 'switched off ' inlet by setting on it velocity u = 0m/s and volume fraction alpha = 0.
As before static contact angle theta0 = 150;
wall
{
type constantAlphaContactAngle;
theta0 150;
value uniform 0;
}


As you can see on the pictures below bubble has been created and simulations converged.







Now, I am sure that my problem has something to do with inlet, but what ? Can anyone tell me what else I could change and how to upgrade my inlet boundary condition to handle wall contact angle 150deg.


To avoid further question my boundary conditions at the inlet are:


0/alpha
Inlet1
{
type fixedValue;
value uniform 1;
}


0/p
Inlet1
{
type zeroGradient;
}


0/v
Inlet1
{
type fixedValue;
value uniform (-1 0 0);
}




Thank you in advance for any help.


Przemek

[PrzemekPL]

Hallo again,

I found temporal solution of my problem.

I've setup contact angle 90 on the walls which are directly connected to the inlet. For the rest 150.
So far it works. I can see nice, rounded bubbles

[duongquaphim]

Hi Przemek,

I am also a new user of OpenFOAM. I worked with segmented flows in a T-junction microchannel as well.

I found that by using the same boundary conditions as yours, at high velocities (more than 0.01m/s) OpenFOAM works well. However, when I set liquid and gas velocity to 0.001m/s, the bubble became smaller and smaller as one of your case (even I already set the contact angle 90 at the inlet and 180 for the rest).

Do you also face this problem? And have you ever try to use dynamic contact angle for this case? Have you ever succeed in obtaining the liquid film between the bubble and the channel wall?

I hope to have much contact with you. It is nice to know someone who use OpenFOAM to solve the same problem .

Regards,

Duong

[Ingenierias2003]

Dear OF users,

I am also a new user of OpenFOAM. I worked with water - air two-phase flow (slug) in many microchannel geometries as well.

From the literature in the microchannel flow the gravity force will not be included in the momentum equations, because only the surface (capillary and pressure) forces are the major.

I am doing a simulation on ANSYS FLUENT 12 from the same case where I can running my case without gravity, and when I trying to compare my solution with OP 1.6 (interFoam), I am not obtaining the same result .
I am trying to use a implicit solver for the gamma equation. I am using constantAlphaContactAngle theta0 90 for the wall of any geometry and not obtaining the same results.

Please anybody tell me if I could deactivated the gravity field on the inteFoam solver or how can improve my case simulation.

Thanks in advance

My kind regards

Ingenierias2003

[sega]

Originally Posted by Ingenierias2003

Dear OF users,

I am also a new user of OpenFOAM. I worked with water - air two-phase flow (slug) in many microchannel geometries as well.

From the literature in the microchannel flow the gravity force will not be included in the momentum equations, because only the surface (capillary and pressure) forces are the major.

I am doing a simulation on ANSYS FLUENT 12 from the same case where I can running my case without gravity, and when I trying to compare my solution with OP 1.6 (interFoam), I am not obtaining the same result .
I am trying to use a implicit solver for the gamma equation. I am using constantAlphaContactAngle theta0 90 for the wall of any geometry and not obtaining the same results.

Please anybody tell me if I could deactivated the gravity field on the inteFoam solver or how can improve my case simulation.

Thanks in advance

My kind regards

Ingenierias2003

As far as I get from the User Guide. You can switch off gravity by changing the file g in the folder constant.
Simply set the values inside to zero.

[Ingenierias2003]

Dear Sega,

Thanks for your help

My kind regards

Ingenierias2003

[Ingenierias2003]

Dear OF user's,


Please anyone tell me if at OP 1.6 which the better schemes of discretization I have to reconstruct the interface when are solving the gamma equation for two-phase flow. I would like to know if OP 1.6 have a similar Geo-Reconstruct or CICSAM scheme discretization implemented on Fluent or maybe have a better scheme.

My kind regards

Ingenierias2003

[ajamy]

Hi all of foamers, i hope that you are well, i wanna to simulate slug flow in vertical pipe, is there any solver released up to now so that completely related with slug flow except interFoam?
tanx

[ajamy]

i find out to use interFoam to simulate 2d slug flow, but when i set a spherical bubble in the below of the vertical pipe, dident happen what is expected. what change or modify be needed to achive correct expected result.
i used this Bc:
____________________________________________

U:
walls
{
type fixedValue;
value uniform (0 0 0);
}

inlet

{
type fixedValue;
value uniform (0 0 0);
}

Gamma:

inlet
{
type fixedValue;
value uniform
outlet
{
type zeroGradient;
}
walls
{
type constantGammaContactAngle;
theta0 90;
value uniform 0;
}

pd:
walls
{
type zeroGradient ;
}

inlet
{
type zeroGradient ;
}
outlet
{
type fixedValue;
value uniform 0;
}
___________________________________________
Result
Attachment 8143Attachment 8143

Attachment 8144

2- my second question is how to create continues slug one after another when i runthe solver?
tanx

[deifobe]

hi, I'm sorry to bother you but i'm working on slug flow simulation in openfoam from more than a month, i don't get the droplet break-up,likely for wrong BC, my dispersed phase stop at the interface between vertical and horizontal arm, any suggestion?
Thanks in advance

[praveensrikanth91]

Originally Posted by PrzemekPL

In my further investigations I've initialized simulation by putting some amount of liquid far away from the inlet. I wanted to check if bubble can be formed from squared shaped volume.
Additionally I've 'switched off ' inlet by setting on it velocity u = 0m/s and volume fraction alpha = 0.
As before static contact angle theta0 = 150;
wall
{
type constantAlphaContactAngle;
theta0 150;
value uniform 0;
}


As you can see on the pictures below bubble has been created and simulations converged.







Now, I am sure that my problem has something to do with inlet, but what ? Can anyone tell me what else I could change and how to upgrade my inlet boundary condition to handle wall contact angle 150deg.


To avoid further question my boundary conditions at the inlet are:


0/alpha
Inlet1
{
type fixedValue;
value uniform 1;
}


0/p
Inlet1
{
type zeroGradient;
}


0/v
Inlet1
{
type fixedValue;
value uniform (-1 0 0);
}




Thank you in advance for any help.


Przemek

Hey,

Am trying to simulate a liquid plug in a capillary and trying to do something like what you did by giving a cylindrical region and letting the contact angle make it into a curved plug but the plug remains as a cylinder in my case. I was wondering if you still by any chance have the case files for this case as it would be a good benchmark for me.

Many thanks