[hilde]

Dear all,
I am modeling a stirred reactor (two phases, water and air, free surface) with a rotating stirrer element in the middle and a cylindrical shaped walls.

The approach used have been to model the entire domain as a rotating domain and the cylinder bottom, top and cylinder as counter rotating walls.

This has felt fine and has given the results wished for once looking at it in post, i.e. the outer walls standing still in the stationary frame and the stirrer in the middle rotating with the same angular velocity as specified for the rotating domain.

However, the thought of the Coriolis and centrifugal forces makes me a bit nervous. I understand the manual as if these forces are added to the momentum equations as momentum sources (as gravity, but different). My worry is then that these forces gives raise to an undeserved acceleration towards the walls of my heavier liquid (water), even if the walls are modeled as counter rotating walls?

Could anyone please comment on this?

(Also, I do want my heavier liquid to be pushed against the walls which is also the results of my simulations, but I do want it to happen because the fact that the stirrer is pushing it outwards)

Additional thoughts:

1. Is it possible to turn off the centrifugal force somehow in CFX 15.0?

2. Is my worry irrelevant? E.g. is the centrifugal and Coriolis forces actually just relevant in the intersection between a stationary and a rotating reference frame? (since I have no stationary frame, just one single rotating)

Thank you in advance and as always is all input helpful

BR

Hilde

[ghorrocks]

The centripetal acceleration creates a pressure gradient from the outer walls in. This is physically correct - that is why the free surface gets a hollow in the middle.

Your fear seems unfounded. The centripetal and coriolis forces CFX applies are real so I do not see why you would want to turn them off.

[hilde]

Thank you very much for the reply. I am however still totally confused about this since I made some trial-simulations to see if the centrifugal force would have any effect.

I did three transient simulations with a cylindrical domain half filled with water, using the free-surface method in CFX 15.0. The k-epsilon method was used, all velocities were initialized to 0 in the stationary frame, gravity was activated and the rotation was set to 1000 rev/min for all cases.

The versions and resulting videos are the following, in where the iso-surface (Air.Volume Fraction=0.5) is shown.

1. https://www.youtube.com/watch?v=e5BE...ature=youtu.be
Rotating domain with counter rotating walls. Cylinder diameter: 2 cm

2. https://www.youtube.com/watch?v=2rNV...ature=youtu.be
Rotating domain with counter rotating walls. Cylinder diameter: 2 m

3. https://www.youtube.com/watch?v=SF9I...ature=youtu.be
Stationary domain with standing still walls. Cylinder diameter: 2 m

(Version 3 was just to make sure there was nothing strange doing on due to initial pressure settings/similar.)

Video 2 is the really confusing one, since is clearly looks like there is some centrifugal force pushing the heavier liquid towards the walls. In video 1 is the same phenomena present, just to a much smaller extent. Speculation: The distance to the rotational axis is not so far so the gravitational force takes over?

Letting 'Simulation 2' run up to 30 seconds does not change the shape of the interface. Also, the attached picture is from simulation 2 and it shows that the walls are actually standing still w.r.t. the stationary frame.

Have you or anyone else any idea what this could be? I am open for the suggestions that I have made an error somewhere, but cannot really see where in that case.

Thanks again

[PeMo]

Sure you get some scaling effects, when you change the diameter and set the angular velocity constant. Try to adjust the rotational speed according to a constant Froude number and the effects should be similar.

[hilde]

Thank you for your reply, and I understand that the cylindrical wall of course has got different velocities dependent on if it is 1 cm or 1 m from the center of rotation.

My concerns is however that there is an effect of fluid being pressed towards the walls even in a case where the outer walls are standing still with respect to the stationary domain.

I visualize this as putting a half-filled bucket of water on the ground and still having the liquid pushed against the walls just because the water molecules think they are in a rotating domain and therefore 'imagines' a centrifugal force?

So my major concerns is the behavior of video 2 and not why video 1 and 2 are not behaving the same.

But thanks in any case and I hope we will be able to sort this out

[ghorrocks]

These simulations do not look converged sufficiently or with adequate mesh refinement to me. So the results are meaningless.

Redo it with a finer mesh and adaptive time stepping, homing in on 3-5 coeff loops per iteration, and make sure you do not hit the max or min limits.