Dear Users I have a case of
I have a case of water jetting out horizontally into air with a very high velocity. The inlet is right on top of a cylinder - see pictures below.
Instead of the water following an almost horizontal trajectory it is turned strongly in a clock-wise direction around the cylinder in the direction of the escaping air - for a bodyfitted grid.
When the cylinder is blocked out in a Cartesian grid the curvature is much less but still present - the water velocity jets out at 1000 m/s - the cylinder diameter is 0.4 meters.
Thus a change in momentum due to the fact that the scalar is convected in the direction of the velocities in the cells - the velocities however being averages for the water-air mixture in the cell. The next picture shows the velocity field after iteration 1 - the downward directed velocity field on the cylinder wall will probably initiate the downward motion of the water:
Is this type of grid dependant behaviour documented somewhere for the VOF method?
The application that I want to model is typical that of milk poured out of a jug and depending on the spout it fans out (spills) or follows a nice clean trajectory into your tea cup.
How could such an application then be solved?
Ps. The solution was not attempted with Foam.
My first thought is that those
My first thought is that those both look like physically reasonable solutions -- you've got something fairly close to a cavitating flow (in the sense that there's a negative pressure on the outside of the cylinder and an optional gas bubble there, though it's air and not vapor), and so both of these solutions might happen in reality depending on whether the air bubble under the stream ends up being present or not. Thus, you've got a situation where there's a bifurcation between two possible flow patterns and thus the system is very sensitive to small changes. Minor changes in the system -- whether in the physical paramaters or in the CFD model -- can easily change the resulting flow from one pattern to the other.
Beyond that, if you look at the cartesian grid, you've effectively got a little stairstep of sharp corners, which in the physical world would be very likely to separate the flow. My guess is that, if you look at the "corner" cells closely, they simply don't have enough momentum going out of the right-hand faces to keep the air from being sucked in by the low pressure.
Thus, my guess is that the body-fitted grid is more accurate for a smooth cylinder. But that's just a guess, and I personally wouldn't trust it without doing some detailed experimental comparisons.
Correctly predicting which of the two flows (attached or detached) will happen is rather difficult with any CFD code -- unless you've done enough experimental comparisons to get a handle on things to the point where you don't need to ask this sort of question, then you've no way to know whether the numerical imprecision is giving you the right flow or the wrong one, regardless of what code you're using.
On the other hand, what you can do is use experimental tests to figure out if the flow is attached or not, and then pick a grid that gives you the same result for that -- in that case, the continuous parts of the solution (that is, the velocity field and such) are likely to be reasonably good.
I have increased the Reynolds
I have increased the Reynolds number through increasing the inlet velocity of the water using 1, 10, 100, 1000, 8000 m/s but with almost now change in the results. I will try tomorrow an experiment using a garden hosepipe and a plastic cylinder.
Thanks for your reply.
Hmm. Yeah, I'd say that if th
Hmm. Yeah, I'd say that if the two grids are giving you those differing results over nearly four orders of magnitude in the nondimensional coefficients, then probably at least one of them is very wrong. It's possible that the flow sensitivity could persist over that wide a range, but surprising.
I'll be interested to hear how the experiments with the garden hose went, and whether you could tell anything about sensivity to conditions.
Another thing that occurs to me to wonder about, by the way: how are you initializing these simulations? If you start one of them with an interpolated flowfield from the other, what happens -- does the attached flow detach, and vice versa?
Hi Brooks Moses I feel quit
Hi Brooks Moses
I feel quit a bit red-faced this morning after doing the hosepipe experiment and then doing similar 3D runs!
I opened the hosepipe (about 15 m/s) over a plastic jar. In the first picture below the water is not touching the jar in order to show its trajectory.
In the following picture the water jet just touches the jar and the result is fanning out of a thin water blade to almost 90 degrees. The top of the water jet trajectory is however the same as the one not touching.
Then I perform a similar 3D simulation. Below the 3D inlet - not quit cylindrical but at least only the bottom part of the jet touches the wall.
And then the result - the top part of the jet's trajectory stays almost horizontal while the bottom half fans out and then breaks away!
Then it was time to perform a sort of a 2D simulation but in 3D - I considered a rectangular inlet but in a 3D mesh:
and to my surprise I got something similar to the experiment - an isosurface from the outside:
and also from the inside:
I believe that there should be good reasons for the 2D case to bend through almost 90 degrees and probably my initial 2D numerical experiment was not realistically defined!
Any comments from your side?
Yeah, I feel like I should hav
Yeah, I feel like I should have thought of that too!
I think you're right that there are good reasons for the 2D case to bend so much -- in 3D, the jet can fan out and become thinner in the crosswise direction, so the bulk of the flow can go straight and the jet can stay attached to the surface simultaneously, so the problems of it having to "choose" one or the other (and the resulting sensitivity to flow conditions) don't occur. In 2D, it can't fan out. (You might get a similar effect in a physical experiment with a jet confined in a narrow gap between two sidewalls.)
This, incidentally, does bring things back to your original subject line -- VOF is known to have strong grid-dependence effects for fluid surfaces that have structure on the same scale as the grid spacing. That's obviously true of pretty much any free-surface method, but VOF has the particular problem that it tends to produce results that subjectively "look right" even when they're completely a result of grid artifacts rather than real physics -- I'm sure you've seen cases where droplets break off that are always about one grid cell across, or sheets that develop holes when they're one grid cell thick. (It looks like this might be happening towards the bottom of your jet in a couple of places, but I can't tell for sure.) I think I've got a good reference on this from a recent conference that I could dig up if you're interested.
|All times are GMT -4. The time now is 05:41.|