I get different results when I scale the 'falling box' tutorial
 

I run the case file of 'falling box' tutorial in which box size and mass is 1m*1m and 666kg. I set the file exactly like instructed in the manual, but the only difference is that I give a downward initial velocity (-5 m/s) to the box through C.G. velocity in 'Dyn. Mesh Zone' window. When I run, the box velocity increases while it's falling and decreases when it's going into water as we expect.

However, when I scale the mesh by a factor of 1/500 (so that box size becomes 2mm*2mm), and I modify the mass and moments in udf, I could see that as simulation runs and box starts falling, the box velocity drops suddenly to ~-1.7 m/s which is not reasonable (the C.G. velocity of box reduces).

Does anyone know what is the reason for this weird behavior of case due to scaling?

PS.
1) I keep the k-eps model for the small box as well.
2) Could it be because of the very tiny values of mass and moment in the second udf? or something related to 'Reference Values' or 'Solution Control' (I've attached the results and both UDFs)

Why does it surprise you? It could very well be that the initial velocity you set is larger than the terminal fall velocity of the reduced box, in which case the drag force is larger than the gravitational pull. Hence the reduced box will slow down. The force balance looks like:

m*a = m*g - 0.5*rho_fluid*v^2*A*Cd.

Your mass goes down by a factor 500^3, while the drag force only decreases by a factor of about 500^2. So in your case it could be that the second term is larger than the first (m*g), hence a decelaration. So I'd suggest to look up for the proper value of Cd for a box, and check the expected terminal fall velocity.

Also, as some alternative tests, try with a smaller reduction and with a reduction of 500 but an initial velocity of 0.5 m/s or even less.

How can I set the Fluent not to consider the drag force only when particle travels in air? (it seems it's not possible just by changing the air viscosity to a very small value)

PS. The reason I chose 'falling box into water tank' is that I think it's very similar to my own problem of droplet-particle collision, and that's why I try to scale it down to my size range.

Then try lowering the density of the fluid, i.e., of air.

I reduced air density and viscosity by a factor of 1e-4. Briefly, with the original mesh, the simulation goes well at the beginning, but eventually particle velocity increases again from -5 to +41 m/s.

But when I apply Dynamic Refinement, as the box approaches the water surface, simulation stops due to some errors although the velocity remains reasonable. What do you think about the reason?
(Please see the attached picture)

Well, I still wonder why you say the -1.7 m/s isn't reasonable when you shrank the box size. Was everything running smoothly in the simulation except for the changed box velocity? If so, let it run and see if the results are reasonable. And try to figure out what the expected fall velocity will be for such a smaller box. I'm not sure of the Cd value of a cube but a quick google seems to suggest about 1-2. So -1.7 m/s of terminal fall velocity in air may not be wrong after all. But again, check it well and try to come up with an estimate.

Then, to reduce your density/viscosity, try to take smaller steps. Reduce it by a factor of 10 and see what the outcome is. Reducing it by such a large factor could introduce all sorts of other problems. So lower it gradually and see. I'd suggest lower the density first, and keep the viscosity (of air) the same.

Another thing that I was thinking about is the box mass that I insert into udf which is originally 666 kg for the large box (1m * 1m). However, when I scale it down (2mm * 2mm), I consider the cube depth to be 2mm and so scaled the mass by a factor of 0.002^3, but I was wondering if Fluent considers a 1m depth and I need to insert the mass for a box with these dimensions: 2mm * 2mm * 1000mm.
I run a simulation with the above-mentioned change, and it seems that the results is much better than what I already got.

In our udf, regardless of the size of the box in X and Y directions, do we really need to insert an equivalent mass for a 1000 mm depth?

hi dear ..
i start working on this tutorial and i cant understand what is the
relation for density and speed and sound. actually i cant understand the physics of problem. i would be very pleasure if u could answer my question kindly,
tanks a lot