pressure on rotating wall
 

Hi,
I am studying lift and drag of a rotating sphere in a shear flow. That's why I am interested in the pressure profile on the sphere. The profile that I get from my simulations looks pretty awkward to me.

I use ICEM to build a blockstructured mesh and convert it to an unstructured mesh to import it into CFX. In the pressure profile you can clearly observe a step in pressure at the edges of the blocks.

I tried several things, like mesh refinement, double precision run, different advection scheme to fix this problem but nothing worked. However, if I set the rotational velocity of the sphere to zero, I get a smooth pressure profile. So, the mesh itself cannot be the problem.

Does anybody have a clue whats going on there?

Any help is highly appreciated!

Yes, I agree your result does not look good. Looks like an interesting problem.

Did you do this using rotating frames of reference? Can you post your CCL file? Also post a cross section through the sphere so we can see the location of the rotating interfaces.

I did this by setting the boundary type on the sphere to wall and defining an angular velocity and axis of rotation.

I hope the cut through the sphere that I did is what you expected. The second attached figure hopefully gives you an idea of the whole problem I am investigating.

Your CCL file looks fine.

Can you post a cross section of the mesh near the sphere? I want to see how fine it is adjacent to the sphere.

Here we go... the first mesh is the one I used to obtained the results displayed in the previous pictures. I assumed that especially the node spacing normal to the sphere surface was to coarse, so I refined the mesh. But the problem remained. The second picture shows the finest mesh I used.

I did the first picture using a plane in CFD-Post to display the mesh. I never did that before. So I did not realize the one line going irregularly through the mesh. If this is not just a display-error, maybe this has something to do with the problem.

The first image shows your mesh to be pretty bad adjacent to the sphere - the elements are tall and thin, where they should be low and flat to get accurate boudary layer resolution.

Your problem is almost certainly mesh size and quality.

Also do a mesh with as close to 1:1 aspect ratio at the sphere surface. This will most accurately capture the near wall effects whcih are the most important in this model.

A mesh with almost cubical cells on the surface was the first thing i tried. The picture below shows the mesh and the pressure profile... unfortunately there is no big improvement.

But even with the coarsest mesh, i still get a perfectly smooth pressure profile if the boundary is not moving.

How are you doing the mesh movement?

The mesh does not move. The rotational velocity of the sphere is implemented setting the boundary on the sphere as rotating wall. The translational velocity is set by assigning a wall velocity in the opposite direction to the tube walls and changing the inlet velocity profile accordingly.

So the whole simulation is pretty trivial. Both velocities are input parameters set by me and are not results of the fluid forces acting on the sphere.

I see. You say you tried mesh refinement, but how fine did you go? You may need to go finer.

The numerics is a bit different for laminar flows compared to turbulent. From memory it includes more of the second order terms from a few parts of the equations - you would have to look through the expert parameters in the documentation to find out exactly which (I cannot remember). But you may need to turn some of them off, or at least to similar settings to turbulent flows. These second order terms may be making it more sensitive to the mesh volume change at your block boundary.

Also, can you try doing this with an unstructured mesh? Do a high quality tri mesh on the sphere, grow out a thick layer of prisms from that, and fill the rest with tets. See if that resolves your problem.

Thanks for ayour help, Glenn. I went really fine. The finest mesh had about 10 000 cells on the sphere surface.

I had a look at the expert discretization parameters. The only thing that I can connect to what you said is the "pressure diffusion scheme".
Also, I tried using first order upwind differencing scheme for the advective terms and it did not fix the problem... so at least the second order terms in the adevection scheme can be eliminated as a possible source of error.

I did the simulation with an unstructured mesh. Except that you cannot see the block edges in the pressure profile anymore, the pressure profile still looks bad, see first picture below.

By the way... if you look closely you can observe a kind of checkboard pattern in the pressure profile. The 2nd attached picture shows one where it is very obvious. When reading through the documentation, I found that this checkboard pattern is typical for bad velocity-pressure coupling methods. Can the pv-coupling have something to do with my problem?

"Really fine" is relative. "Really fine" on a desktop PC is just a quickie for a super computer. Can you post a cross section of the mesh of this really fine mesh? Make sure you get the mesh right next to the wall.

Yes, the checker board pattern is a sign of P-V coupling issues. This is very uncommon in CFX, the default PV coupling is normally very good.

What is the aspect ratio of the elements near the region which is showing the weird pressure area?

My finest mesh has about 50 000 cells on the sphere and 5 million in total (on a not-rotating sphere, i obtained physical results with about 3000 cells on the sphere or even less). The aspect ratio is about the same for all cells on the sphere, and in this case it is in the magnitude of 1.

The results of the run with this mesh are shown in the attached picture. The fine mesh did not exactly fix the problem but gave me a beautiful color pattern. :D

I suspect that mesh quality is your issue. On two fronts:
1) Your elements have internal angles approaching 45°. I would try with 1:1 aspect ratio elements with just about 90° angles. You can do this by doing inflation on the sphere rather than the block structured mesh you currently have.
2) Your elements expand away from the sphere too fast. For accurate results use an expansion ratio of 1.01-1.02. Yours looks much higher than this.