meshing a sphere - large deviation from perfect sphere
 

Hi,

I am simulating a laminar flow around a rotating sphere using CFX. However I get an unphysical pressure profile on the sphere, see first attached picture. The pressure profile is wiggly and shows steps at the block edges.

After weeks of troubleshooting, I was finally told by the ANSYS CFX support that the reason (at least for the wiggles) is definately the irregular (-> non-spherical) shape of the sphere. However, I am not able to obtain a sufficiently spherical surface.

I use a blockstructured mesh created in ICEM. The sphere is created using the option Geometry -> Create surface -> standard shape -> sphere. The blocking strategies that I tried are shown in pictures 2 and 3.

I am aware of the fact that I cannot create a perfect sphere using linear elements. However, for two reasons I do not think that the linear approximation is the reason for the deviation:
1. when refining the mesh, the amplitude of the deviation should decrease. but it does not, see picture 4.
2. In case ICEM places the nodes on the radius specified by the geometry, all nodes are supposed to have the exact radial position. In case ICEM places the center of the elements on the radius, all nodes should have a radial deviation in the same magnitude. Also the deviation should probably be positive, so the nodes lie outside the sphere ı guess.

So, how do I get ICEM to create a spherical mesh?

how does the mesh inflation look coming off this sphere? ensured everything is uniform?
just throwing out ideas/questions.

Another way to look at it, your nodes are on the surface but what about the face center error/deviation from the surface?

What exactly do you mean by inflation coming off the sphere?

If you are refering to the node spacing on the edges that come off the sphere, then yes - they are uniform. Especially in the case of the first blocking. Here the sphere is in the center block of an o-grid. So alle the edges goind outward have the exact same spacing.

I agree with you on the face center deviation. It seems as if ICEM puts the node on the spherical geoemtry and linearly connects thos nodes to form the face. This means the face centers are always located inside the acual sphere. This correlates with the fact that "radius range" calculated for the boundary ?(nodes/elements)? is 4.997 to 5 where the perfect sphere has a radius of 5, see last picture attached to my previous post.

However you can see agglomerations of adjacent nodes elements lying considerably inside the sphere while at other regions there are several adjacent elements exactly on the right radius of 5. So there must be some other error than just the deviation of the face centers due to the linearization of the surface.

I think he was referring to the wall-normal resolution of the mesh.
What Yplus values are we dealing with? could you show a cross-section of the mesh?

Yet another thought: did you associate the faces correctly to the geometry? Or did you rely on the auto-association?

The wall normal resolution is uniform due to the blocking topology.

I cannot tell the y+ value from my mind since I was not aware that it is important for laminar flow. I attached cross sections of two of several meshes that I checked.

Mesh refinement (also in the wall normal direction) does _not_ positively influence the pressure profile. A mesh morphing in CFX that moves all elements to the radius of the perfect sphere does.

So, my question is: Is there a way to get ICEM to generate a more spherical sphere?

I associated the edges to the surfaces.

Interesting.

Attach tetin (.tin)

Would it help to assign the faces of the blocks to the surfaces?

I was able to drastically increase the accuracy of the mesh by setting the "project to Bspline" option in the meshing options. The radius range of the surface elements is a lot smaller now, see attached picture.

This removed the checkerboard pattern in the pressure profile! However the steps at the block edges are still observable. Just as the radius of the sphere surface elements still seems to have a little step here.

- I attached the .tin file --> zip file.
- Assigning the faces to the surface did not have any effect.
- The y+ value for the case i took the attached pictures from is y+=0.05 (taking the highest Wall Shear occuring on the sphere for calculation of the fricting velocity)

I just set up a simple test case with a rotating sphere in a flow field with ICEM and fluent. Didn't meet any of the problems you encountered.

Thanks for all the effort!

I actually already tried to do the simulations in FLUENT because of that problem. But I had the same situation in FLUENT.

Can you check the shape of the sphere in FLUENT like shown in some of my pictures? I mean a simple expression/UDF: radius = sqrt((x-x_c)^2+(y-y_c)^2+(z-z_c)^2) where x/y/z_c are the coordinates of the sphere center.

Again, you are helping me a lot! Danke :)

Here you go.
The deviation in the radius is about 0.5%, more than I expected.
Nevertheless, the results for pressure look quite ok.
The calculations were run in fluent, i just used the CFX result viewer because it is awesome.
Rotational axis in my case was Z.

I suspct that problem was due to blocking approach.

Alex: This is strange... I have to think about that. Whats the angular velocity of your sphere?

Far: You can see two different blocking strategies that I tried in the pictures attache to my first posting. The worst element quality is in all cases between 0.6 and 0.8. What do you think is wrong? - EDIT: Since you cannot see the geometry in the pictures, I should mention that the sphere is located in a pipe/cylinder. That is the reason for the o-grid.

Inlet velocity in my case was 1e-4 m/s.
Angular velocity was 1e-4 rad/s.
Fluid was "Air".
Diameter of the sphere was 2m.

How high is Re in your setup?

The pipe Reynolds number in the case is 100. However i investigate the range of 1 to 100 and I get the same problem for all Re.

As far as the sphere reynolds number is concerned things are more complicated. The sphere is moving with the flow (implemented by moving the pipe wall in the opposite direction). Taking the relative velocity of sphere and the velocity of an undistrbed parabolic profile for calculation of the particle Reynolds number, I get Re_p = 0.16.

In contrast to your simulations, I use the property data of water except for a higher viscosity. The relative velocity of sphere and fluid is 5e-3 m/s while omega*r_sphere is 3e-2 m/s. If you have time to change your simulation to these velocity ratio and check it out again that would be great.

The results are still plausible without the dubious pressure distribution on the sphere that you observed.

Your rotational velocity is about one order of magnitude higher than the fluid velocity. Are you sure that the flow remains laminar in this case?
I did my simulation in steady-state which was only possible when I increased the viscosity of water by an order of magnitude.

Yet the pressure pattern on your sphere is a different issue. I suppose it comes from your blocking strategy.

My strategy would be the following:

1. create 1 block for the whole channel
2. create an o-grid for the walls of the channel
3. make 2 splits, one before and one after the sphere to get a nearly cubic block around the sphere
4. create another o-grid of the center block which encompasses the sphere (ONLY this one block)
5. Delete the center block of the newly created o-grid
6. Assign the faces of the blocks around the spere to the surface of the sphere

I am absolutely sure it stays laminar. For the sphere, the creeping flow assumption ist almost applicable.

The blocking strategy that you described works fine if the sphere is in a square. In my case, the sphere is inside a round pipe and with this topology I get bad quality elements... I will do this blocking and post a picture in a few minutes, so you can check if I understood you correctly.
EDIT: You were right. I was wrong. The element quality is fine :) Now I'm curious about the pressure profile....

Aaah you just made my day ;)

there you go... the new blocking and pressure profile. still sudden pressure changes at the block edges. any other suggestions?

i know you don't expect the radial deviation of the surface elements to be the reason. but one thing is interesting: only the elements lying on the two sides that are facing the flat inlet/outlet have a significant deviation. the other four side that are facing the round pipe wall are perfect.

Well, same thing in a round channel.
The pressure on the sphere looks ok. Yet it is clearly visible that I should have created the mesh with a lot more patience.

Are you sure that you carried out step 6 correctly using the "associate face to surface" option?