Learning Forum

[BillT]

Hello,

I am modeling a 2d multiphase flow (air and water) with gravity enabled in negative x- and y-direction. It seems that the water flows along the wall, even though the gravity is greater in y-direction (see below). The area is filled with air. Did I forget to disable any kind of wall adhesion? If I increase my velocity at the inlet, it doesn't flow along the wall.

Some Boundary Conditions:

   Gravity: x: -4.25 m/s² ,      y: -7.3575 m/s²

   Velocity at inlet (Volume fraction of water = 1): -0.01 m/s

            

Thank you in advance!

 

[Rob]

Please can you plot the phase contours & add them into the thread. I wonder if you've missed something in the boundary setting for the outlet, but equally it could be convergence so please also add the residual plot.  

[BillT]

Below you can see the settings for my pressure outlet, the residuals and the contours of the water volume fraction. It seems like there is not much water in it. 

[raul.raghav]

BillT, its still not clear where your different boundaries are located. Can you provide a detailed schematic which describes the different boundaries? Which is the inlet, outlet, wall? And provide a schematic of the coordinate system as well, so that we could understand the problem.

[BillT]

Here is a small sketch of my geometry and my boundaries.

[Amine Ben Hadj Ali]

Please paste a contour of Volume fraction (filled). From the first image one can (hardly) identify that water is flowing along the top wall in -X direction and then towards the -Y direction as it is expected if gravity is enabled and due to buoyancy. Just give proper operating density: give 0 kg/m^3 and set pressure outlet to the pressure outside the domain ( I think ambient). 

[raul.raghav]

Something seems to have gone wrong in your setup with the boundary conditions. 

Could you attach your workbench archive file? Please follow these directions to upload a .wbpz file.

[BillT]

Sorry for my late response. When I activate filled for the contour of my volume fraction it doesnt show any difference. But I set the range of water volume fraction from 0.01 to 1 (see below). How do I set pressure outside the domain to ambient? Shouldnt it be the same as setting the gauge pressure to zero?

[raul.raghav]

I looked at your files and everything looks fine to me. The -X direction gravity is high and the Y direction velocity is low, so what you're seeing in physically possible. I don't think there is anything wrong with the setup. However, there is one thing that you need to be careful about. There is reversed flow at the outlet and this could influence the results. I would extend the outlet such that it further away from the inlet. Then trying running the simulation again. Let us know how that goes.

[BillT]

I appreciate that you looked at my files. When I put the outlet further away from my inlet it doesnt change the reversed flow issue. But I set the wall at the top of my boundary to pressure-outlet and it works fine.

Thank you for your help.

BillT

[Rob]

As an aside, don't select any surfaces when plotting contours in 2d. You'll have much clearer graphics. 

[raul.raghav]

Out of curiousity, can you attach a figure of the velocity or volume fraction contour after you set the top-wall to pressure-outlet?

[BillT]

This is a slightly modified geometry, but the same result.

[Rob]

You've got a couple of problems here. The first is there isn't enough mesh to retain the water phase in the domain: it's diffusing out so your result won't be accurate. The second issue is that the air flow may be strong enough in 2d to deflect the water: can you plot (with filled contours) the velocity?

[BillT]

Here you go.

[Rob]

Thanks. If you compare the mass fraction & velocity plots you're getting a very diffuse jet and that's causing problems with the numerics.  Please can you adapt the region where the water is and continue the solution. You may need to do this a few times, so I'd also advise increasing the resolution on the original mesh: you're aiming for 10-15 cells across the water jet.