[Jack_Landis]

Dear foamers,


I'm dealing with a two phase flow (water and air) using interFoam. Water flows through a duct in a chamber and then exits the chamber via another duct. The chamber has been depressurized to few mbar, so the fluid moves because of the difference of pressure.


And here comes my problem: I tried fixedValue for pressure inlet and outlet and, as I read in the forum, it doesn't converge. Then I tried a totalPressure inlet, but again very slow convergence and very small time steps (10-90 or so).


Now I am wondering: how can I impose the pressure difference between inlet and outlet? I need to play with this value in order to understand the order of magnitude of the depressurization I must create in the chamber for my purposes.


Thank you in advance,
Jack

[gkarlsen]

Originally Posted by Jack_Landis

Dear foamers,


I'm dealing with a two phase flow (water and air) using interFoam. Water flows through a duct in a chamber and then exits the chamber via another duct. The chamber has been depressurized to few mbar, so the fluid moves because of the difference of pressure.


And here comes my problem: I tried fixedValue for pressure inlet and outlet and, as I read in the forum, it doesn't converge. Then I tried a totalPressure inlet, but again very slow convergence and very small time steps (10-90 or so).


Now I am wondering: how can I impose the pressure difference between inlet and outlet? I need to play with this value in order to understand the order of magnitude of the depressurization I must create in the chamber for my purposes.


Thank you in advance,
Jack

Not sure I understood your case, but it sounds like you are confusing p_rgh with pressure (it's not the same thing). You might want to take a look at the boundary condition prghPressure if you are trying to set a static pressure and calculate the flow.

[Jack_Landis]

I am sorry, I didn't mention the difference. I set bcs for p_rgh and I want to simulate a flow due to a pressure difference. I tried the bcs I explained before but they doesn't work...What could you sugest me?

Thank you!

[gkarlsen]

If you already tried the boundary condition I refer to in my previous post (prghPressure) to no effect I think you need to provide more information. Preferably by sharing your entire case, but at least the content of U, p_rgh, and alpha files

[Jack_Landis]

I tried the bc you suggested me but still I have problems: the time step is refined until 10^-100 and then the simulation crashes…I share with you the files I used, could you please have a look at them?

Thank you in advance!


alpha.air.c

p_rgh.c

U.c

[Jack_Landis]

I'm sorry, I posted the wrong p_rgh file... Here is the one I used!p_rgh.c

[gkarlsen]

I understand that you are trying to simulate some sort of chamber/plenum with multiphase water/air flow, a inlet and a outlet, and a given differential pressure between the two. Since you did not provide a full case file, I created a simplified version which consists of a 0.5x0.5x0.5 m cube, a vertical submerged inlet from the bottom with diameter 50 mm and a horisontal discharge with diameter 50 mm. It looks like the attachment after 2 seconds of time simulated.

I used 1000 Pa total pressure in the inlet in the bottom left, and 0 Pa in the outlet to the right. I used prghTotalPressure BC, but could have used prghPressure if you just want static pressure.

U

    walls
    {
        type            noSlip;
    }

    inlet
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    outlet
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }

p_rgh

    walls
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    inlet
    {
        type            prghTotalPressure;
        p0              uniform 1000;
        value           uniform 1000;
    }

    outlet
    {
        type            prghTotalPressure;
	p0		uniform 0;
        value           uniform 0;
    }

Full case can be found here:
https://drive.google.com/file/d/1mtO...ew?usp=sharing


Also, you might want to take a look at this post:
How to give enough info to get help

Good luck

[Jack_Landis]

I tried with your bcs and it works! Now I'll try with the static pressure, that is what I need.

Anyway, I attach you the files of my simulation and a video of the results...Initially everything seems meaningful, but after a while something strange happens...I think not physical fluctuations due to contact angle/surface tension, and air appears somewhere in the liquid phase...May you have a look please?

You can find all the files here: https://drive.google.com/drive/folde...US?usp=sharing

[sumitzanje]

Hi all,

Im trying to simulate the pressure-driven two-phase flow. The best example is underground sewer tunnels.

I have an inlet pressure of 115020 N/m2, and outlet pressure of 114876 N/m2. (consider these pressure for the sake of discussion).

The distance between the inlet to outlet is say 35m, and at a distance of 25m from the inlet, a vertical pipe of height 6m is provided.

Initially, the horizontal pipe is flowing full, with the vertical pipe is partially filled. This simulation is allowed to run till a steady state is reached.

Now an air tank is introduced to the horizontal pipe, in between the inlet and vertical pipe.

The pressure of air is assigned such that it allows smooth entrance of air to horizontal pipe, and it keeps advanced towards the vertical pipe.


My simulation is crashing as air also advances towards the inlet, and it reaches the inlet patch. The air has lower pressure than the inlet patch, and I feel that is causing some problems.

Inlet Patch BC's:

inlet
{
alpha
{
type fixedValue;
value uniform 1;
}

p_rgh
{
type prghTotalPressure;
p0 uniform 114766.94;
}

U
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}

T
{
type fixedValue;
value uniform 293;
}

k
{
type fixedValue;
value uniform 0.000188139;
}

epsilon
{
type fixedValue;
value uniform 4.34537e-05;
}

omega
{
type fixedValue;
value uniform 0.1;
}
}


Outlet Patch BC's:


outlet
{
alpha
{
type inletOutlet;
inletValue uniform 1;
value uniform 0;
}

p_rgh
{
type prghPressure;
p uniform 114442.0;//102424.6804 (wrong)
}

U
{
type inletOutlet;
inletValue uniform (0 0 0);
}

T
{
type inletOutlet;
inletValue uniform 293;
value uniform 293;
}

k
{
type inletOutlet;
inletValue uniform 0.000188139;
value uniform 0.000188139;
}

epsilon
{
type inletOutlet;
inletValue uniform 4.34537e-05;
value uniform 4.34537e-05;
}

omega
{
type inletOutlet;
inletValue uniform 0.1;
value uniform 0.1;
}
}



Air Tank BC's:

tank
{
alpha
{
type fixedValue;
value uniform 0;
}

epsilon
{
type fixedValue;
value uniform 4.34537e-05;
}

k
{
type fixedValue;
value uniform 0.000188139;
}

omega
{
type fixedValue;
value uniform 0.1;
}

p_rgh
{
type totalPressure;
p0 uniform 114298.0;
}

T
{
type fixedValue;
value uniform 293;
}

U
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
}


Please advice. What could be an issue?


The 2D simulation with the same BC's is working but the with 3D case it crashes after 32sec, and this is the point when air from the air tank reaches the inlet boundary patch.