[Andrea_85]

The tutorial "capillary rise" of interfoam uses two pressure bc at inlet and outlet, flow is driven by hydrostatic pressure (and capillary forces) and it works fine. If you have only 1 phase at the boundaries i think there is no problem. If you have 2 phases in contact with inlet or outlet then it becomes more tricky.

Best,
Andrea

[Saideep]

I tried to replicate as close as to capillaryRise case.
It looks to get some shape but still there seems to be some problem.

I used the following bcs: {2D case and no influence of 'g'.}
P_rgh {inlet: 500Pa, outlet:0Pa, fixedWalls: fixedFluxPressure}
U {inlet/ outlet: pressureInletOutletVelocity, fixedWalls: (0 0 0)}
Alpha {inlet: inletOutlet {based on phase number for value}, outlet: zeroGradient, fixedWalls: equilibrium ca of 30}.

Everything looks fine until the drop/ bubble flows out of the channel. Soon there is a change in the phase representation. That is if i have a water drop passing out of the channel the channel is being filled by water and air starts to displacing from the inlet again. See pictures 1 and 2 (successive time steps data with the provided bcs). This looks quite nonphysical. How can water enter the system? Any ideas over this.

Thanks;
Saideep

[Andrea_85]

Not sure i have understood well your problem. I don't think the 2 pictures are successive time-step since in the first one the water bubble is still far from the boundary. Try to put fixedvalue 0 at inlet for alpha. Which version of OF are you using?

Btw, as i said before, at the breakthorugh you have multiple phases on the outlet boundary and the constant pressure bc might be no longer correct.

best,
andrea

[Saideep]

Thanks Andrea,

Sorry I was not clear in my previous post. I am using OF2.3.1. In my bcs for alpha i mention alpha(0-> air) injection at inlet and zeroGradient at outlet.

As you mentioned earlier, specifying fixedPressure at outlet {along with the inlet face pressure} seems not a good option. Attached are two time steps with glyphs just to be clear what is happening within the system.
fig0.jpg

fig1.jpg

To adjust pressures at inlet and outlet to fixed values, a pressure gradient developed is causing backward flow possibly.

So, is fixing the inflow at inlet and fixing pressure at outlet only solution?

Saideep

[Andrea_85]

Can you show also the pressure field of those 2 pictures.
or alternatively, if you provide the test case i can give it a try.

andrea

[Saideep]

Attached is the test case.

Best;
Saideep

channelFlowFixedP.zip

[Andrea_85]

Ok, now i see what is going on.
Your channel is very small (R=2.5 micormeter) and capillary pressure is very large. If you don't provide a pressure force (between inlet and outlet) larger than the capillary force (which points to the negative x-axis after the first meniscus has left the domain) you will have flow from right to left (negative x-axis). Note that when the bubble is full inside the domain, the total capillary force is approximatively zero (if you assume that the 2 menisci are perfect circles) and the bubble moves correctly from left to right.

Just check the forces (after the first meniscus has left the domain).

-capillary force
Fc = gamma*cos(theta)*L = 6e-7 N (L is lenght of the contat line)

-pressure force
Fp = deltaP*A = 1.25e-8 N (A cross-sectional area of the channel)


There's nothing wrong with your simulation

Best,
Andrea

[Saideep]

Thanks for that explanation Andrea.

I just made the case more complex, {plus channel}: instead of fixing pressures at inlet and outlet, I now try to inject at constant rate(water displacing air) and have fixed Pressure at outlets.

In figa, you can see injecting water (left face inlet and all remaining faces are outlets) into the system. In figb, i guess the capillary force that spread out into the top and bottom channels is balanced but there could be capillary force acting normal at the junction point which is acting along the direction of the pressure force.

I am confused of what is causing air to flow into the system from the outlet face on the right side? {figb}

figa.png figb.png

In figc, as you mentioned there is a two phase outflow and is defining fixed pressure bc a good option? I am just wondering how can water flow inwards from the outlets{top and bottom faces} for this case. I am using pressureInletOutletVelocity which is like a zeroGradient for outlet for U as bc for outlets.
figc.png

Best,
Saideep

[Andrea_85]

Try using inletOutlet for alpha with inletValue 0 (which is air in your case if i am not wrong) instead of zeroGradient to prevent water coming in from the top and bottom boundary and yes, in my opinion, it is not a good idea fix the pressure on those boundaries. I would fix it on the right boundary where you have only 1 fluid.

Best,
andrea