Hi,

I want to address a problem that have been giving me headaches for some time now. If I try to simulate a fluid (e.g. water) injected between two parallel plates to replace another fluid (air) in CFX, the flow front do not look good at all.

This problem actually has an analytical (quite complex) solution in the limiting case where the air has zero viscosity and the plates are infinitely long.

European Journal of Mechanics B/Fluids 23 (2004) 571â€"585

The homogenous CFX solution look very different from this. It seems as if the triple point (where water air and wall meet) is not moving in the flow direction, there is only movement of fluid in the middle of the gap between the plates. The problem is also described in Rui Igreja's master thesis:

http://RuiIgreja.googlepages.com/Rui...sterThesis.pdf

The inhomogenous solution look a bit better. Is it really not possible to simulate such a problem using CFX?

Thank you for your comments!

- Terje

The last question should be

Is it really not possible to simulate such a problem using the homogenous model in CFX?

Hi,

I have had a quick look at Rui's thesis from your link. I do a lot of free surface work lately so I have a few ideas of what helps them along. I cannot see the EJFM reference.

It is concerning that the liquid phase does not contact the wall, I have never seen this before.

But one thing I notice is that Rui is using quite high aspect ratio elements, and with the elements being squished into the boundary layer the aspect ratio of the elements here are even worse. In my experience free surface with surface tension need grids with aspect ratios close to 1 for accuracy. I don't think Rui used surface tension but I would be interested to see what happens if that model is repeated with aspect ratio 1 elements.

Hello Rui, are you there? Any comments?

Regards, Glenn

Hi,

I should also add that there is a known failing of the Navier Stokes equations in that they are undefined at moving contact lines. The essence of the contradiction is that a moving contact line requires fluid to move along the wall boundary to get the line to move, but the no-slip condition says fluid cannot move along a boundary. The Navier Stokes equation breaks down here and it is an area of active research as to what to do about it.

Most CFD codes ignore this problem and somehow (I don't fully understand how) things seem to work OK. Maybe you have found a case when you can't just ignore it and you have to do stuff like making the wall a slip boundary for one phase a slip, as Rui did - and this means you need an inhomogeneous model.

Glenn Horrocks

Hi,

Thanks a lot for your comments Glenn! The failing of the Navier Stokes equations also leads to a singularity in pressure at the triple point. As you point out this is a very plausible reason to why the homogenous model fails to provide the physical solution. Specifying both a finite viscosity and no-slip at the wall is not associable with a progressing flow front.

The reason for the artifact in the solution is not a skewed mesh as used in the master thesis. I have tried with several meshes, also very fine ones and refined near the wall but the problem persists.

Using the inhomogenous model with no-slip/no-slip conditions also leads to unphysical effects in my experience. The flow front breaks up and forms feathers.

The best solution as I see it is using the inhomogenous model with no-slip conditions for the injected phase and complete slip for the displaced phase. This is, however, computationally quite expensive and I hoped with the previous post to find a way to avoid the problem.

Best regards Terje

Hi,

CFX V12 is currently in beta testing. It would be good to run this as a test case on V12 and hopefully with a bit of work on the software the issue can be fixed for the next release. I would talk to your CFX rep and ask to test your case on V12.

Regards, Glenn

Hi Terje and Glenn,

Here are some results I got some time ago. The geometry is being filled with a liquid from left to right, the gravity vector is from right to left (-9.8,0,0). The gap between the top and bottom walls is 3.2 mm, and the average inlet velocity is 0.1 m/s (imposed with a parabolic profile).

The 1st figure shows the results obtained without Surface Tension, the 2nd one results with Surface Tension (Coefficient=0.07 N/m, approximately the same as water-air):



You can see that, despite the elements aspect ratio being close to one, and the mesh good enough to capture reasonably well the interface, the problem of the liquid phase not contacting the wall also happens. The results obtained with Surface Tension seem a little bit better, but I think that is just because the surface tension force acts to reduce the interface curvature and to make it round.

In my thesis I didn't use Surface Tension, because 1) I thought it wasn't important for what I wanted to get from the simulations (I wasn't interested in the detailed interface shape), and more important 2) I didn't have any data about the surface tension coefficient, neither wetting angle, for the liquid (a thermoset resin) I was using.

The reason for this wrong behaviour, at least in my point of view, is that the physically correct no-slip condition on the walls, doesn't let the air to move away to give place for the liquid. It is written in my thesis that this had already been mentioned by some authors. But why is reality different? In my opinion it is because reality is a continuous world, not a discrete world. It's the same as Achilles being unable to reach the turtoise. In Fig.7 of my thesis it's shown that increasing the number of mesh elements in the gap direction reduces the size of the layer of air between the liquid and the walls. Although, the volume fraction of liquid on the wall nodes decrease.

However, on the other hand, if the mesh elements close to the walls are big enough this wrong behaviour won't be noticed. And I think that's why Glenn and most of people don't see this happening, they don't use (and probably don't need) that fine elements close to the wall, and probably explains Glenn commentary "Most CFD codes ignore this problem and somehow things seem to work OK" On the next 2 figures, you can see the results from a 3D mould simulation. The 1st figure shows the volume fraction on the thickness direction (with small elements size), and the 2nd figure the volume fraction on the symmetry plane: <A HREF="http://img134.imageshack.us/img134/8410/symplaneqr4.png" My interpretation is that when the mesh elements size perpendicular to the wall is big enough, because the velocity on a wall node represents the average velocity of the control volume surrounding that node and not the wall velocity ("conservative" velocity on a wall node is not zero), the air will be able to move away. So, Glenn, I think if in your simulations you had small elements close to the walls you'd also see the behaviour we're talking about.

I also did some simulations where the moulds were being, instead of filled, emptied of liquid. This can be regarded as a mould initially full of liquid being filled with air, and you could see a similar behaviour. But in this case, if you are interested in what happens to the liquid, you cannot apply the free-slip condition to the liquid. But as this situation wasn't the objective of my work, I didn't play with it for very long.

P.S.: Terje, I asked you a few questions on a reply to one of your posts (<A HREF="http://www.cfd-online.com/Forum/cfx.cgi?read=28667">http://www.cfd-online.com/Forum/cfx.cgi?read=28667 </A>). Could you take a look?

Rui

Hi,

Thanks you the detailed comment Rui.

I do not see the air layer you talk about and am certain that I will not get it in my stuff. I looked at capillary driven flows so if the liquid does not touch the wall then there is no driving force! In your case the flow is driven by a pressure source pushing the flow forwards.

Interesting how even though both cases have moving contact lines, capillary driven flows are OK but your pressure driven flow shows a spurious air layer.

Did you include a wall wetting angle with surface tension in your stuff Rui? That may cause the liquid to stick to the walls and the air to form small bubbles on the wall. Could this be what physically happens?

Glenn Horrocks