[ghost82]

Hi all,
I have some questions about a test case I'm running.
The case is very simple: a cylinder (radius=5 cm, height=1 cm, positive Z), filled with water, rotating at 105 rad/s around Z axis; cylinder is centered in 0,0,0.

I'm using fluent to evaluate results.
I thought that single reference frame, moving mesh and moving wall (set up in the wall boundary panel) simulations should give similar results.

Instead, I got similar results for SRF and moving wall, but not for the moving mesh..
Can anybody explain why?

I'm attaching velocity contours in xy plane, at mid-height of the cylinder, cell centered values, (variable velocity for fluent, velocity in stn frame for cfd-post) for the three cases.

Daniele

[JBeilke]

This is a nice testcase for the moving mesh implementation :-)

Unless you specify the motion of the wall to be rotation, the fluid should stay in rest.

When dealing with moving meshes you also have to take into account the "space conservation law" (Raumerhaltungsgesetz).

[ghost82]

Strange thing to me is that in the moving mesh case I specify both the motion of the mesh and the absolute rotational velocity of the walls... (I did 2 tests, the first with relative motion, 0 rad/s relative to adjacent fluid zone and the second with absolute rotational velocity, 105 rad/s, but results are the same)..so I don't understand why the fluid seems stationary...

[JBeilke]

For moving mesh cases you might get 2 different sets of velocities for postprocessing -- absolute and relative velocity. Did you check this?

[ghost82]

Yes, I checked in cfd post because fluent has only 'velocity magnitude' (and it should be absolute vel.). In cfd post velocity in stn frame should be the absolute velocity (equivalent to velocity magnitude).
Moreover, all results were compared with ensight and I chosed the same velocity variable for all the cases.

[lovecraft22]

I don't have any experience with fluent so I may be completely wrong here.

Usually, moving wall and SRF (I'm assuming it's the same thing as a MRF) can be used with both a steady state (a RANS for instance) and transient simulation (a DES for instance).

On the other hand, a sliding mesh would make sense for a transient simulation only although in your case the geometry position would no change in time for a fixed observe, being your cylinder completely smooth.

Did you run a transient simulation for the sliding mesh? If yes, did you run for long enough in terms of physical time (seconds)?

[ghost82]

Thanks for reply. Yes, moving mesh test case was run in transient, for 1 second, starting from the srf solution.

[ghost82]

It seems the problem was the timestep: I didn't check the timestep independence and I set up a timestep so that 100 timesteps were needed to complete a revolution.
Even if the solution converged (continuity residual below 1e-4, below 1e-5 for others) and the area weight average velocity magnitude did not change vs physical time on the xy z-mid-range plane the result was not true.

Timestep of 1e-4 was needed to have a solution independent of the timestep (this means 600 timesteps per revolution!!!!).

[JBeilke]

Thats why it is a common practice to do a steady mrf run for the initialisation :-)

[ghost82]

Sure, however, even if the solution is initialized with the mrf solution, and you don't set a correct time step (and the only way is to perform a timestep independence study) results will be wrong as the solution tends to go always to 0 velocity.

[CeesH]

600 timesteps, that's quite a steep requirement. Especially for a case that looks so simple. Nice test!

[Alex C.]

Hello,

It is indeed a nice test that you are performing.

I can't help but find that the plot that you posted seem quite different one from the other.

You should consider plotting along the radial direction, and overlay the 3 result curves.

I also suggest that you plot for velocity component instead of magnitude. Again, I would plot radial velocity and tangential velocity along a chosen direction.

[JBeilke]

It sounds very strange that the velocity should go to zero when using a too large time step. So I tried it myself with CCM+ and was able to specify timesteps as large as 600 degree/step without problems. It requires some more inner iterations but there is no sign that the velocity goes to zero.

[calv]

Hi,

Sorry to bring up this old post, but I am just wondering with your rotating cylinder, shouldnt the velocity near the cylinder wall close to zero/small number?

It should be vel -> 0 near wall then higher velocity and then slower velocity as it approaches the centre? Is that right?

[ghost82]

If you speak about absolute velocity, no: the wall of the cilinder is rotating!

[calv]

Originally Posted by ghost82

If you speak about absolute velocity, no: the wall of the cilinder is rotating!

Thanks for the reply! Oh stupid me that make sense! The cylinder is making the water rotate.

Actually the reason I asked about this is that I have a recent post similar to this cylinder problem. Instead, I have a rotating propeller and I am a bit confused about why I have max velocity at the propeller wall boundary in the stationary frame, and only in the local/rotating frame, the velocity at the propeller wall boundary -> 0. I am still a bit confused about my case, could you please help me ? Sorry i am not sure if I am supposed to redirect post like this, new to this forum.

Thanks,
Calvin

[agd]

If I understand your question, in the rotating frame the velocity of the fluid relative to the propeller should be zero at the propeller surface because you have the no-slip condition. The fluid has to move with the solid boundary there.

[calv]

Originally Posted by agd

If I understand your question, in the rotating frame the velocity of the fluid relative to the propeller should be zero at the propeller surface because you have the no-slip condition. The fluid has to move with the solid boundary there.

Thanks agd, it kinda make sense to me now.

[damon707]

Hello all,

Continuing the discussion about rotating reference frames, I want to simulate a wind turbine rotor (blades and hub only) with SRFSimpleFoam. Currently I have a cylindrical computational domain as shown in the picture.The radius of the rotor is R=1.19m and the radius of the cylindrical domain is 5R.
I cant get a physical solution. I get a converged solution but the result is quite unphysical, there is not even a wake formed behind the rotor. Is this wrong result due to the size of the cylindrical computational domain? Where can I find info on how exactly the size of the domain affects the accuracy of an SRF simulation?

Best,
George