CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Meshing a centrifugal compressor impeller (http://www.cfd-online.com/Forums/ansys-meshing/85344-icem-meshing-centrifugal-compressor-impeller.html)

Mitpostdoc February 23, 2011 12:57

[ICEM] Meshing a centrifugal compressor impeller
 
Hello there,
I am experiencing a lot of difficulties in meshing a centrifugal compressor with Icem.

The geometry is essentially a centrifugal compressor with backward-leaning impeller and vaneless diffuser. I can not use a structurate grid because of the complexity of the structure.

I must construct a mesh only of a single passage/vane... However, any attempt I made to make Icem understand the geometry and use the unstructurate mesh generator on a single vane has failed miserably :(. The backsweep angle is something which ansys is unable to understand. I am trying to define a periodicity in the global mesh parameters and I am specifying the correct angle or number of sectors. Icem is just meshing everything in an angle without understanding that the impeller blades iare bending backward.

Is there any way I can define periodic boundary conditions on this kind of geomwtry?:confused:

I hope I have been clear enough, and I thank you for your help!:)

Will Anderson February 23, 2011 13:51

Please post pictures, screenshots, etc.

I recently meshed a centrifugal compressor, at the beginning I was using periodic boundaries, but I eventually went with a full 360 domain as my flow was non-periodic anyway.

Mitpostdoc February 23, 2011 16:30

Thanks for the fast reply ;). Please, look at the following sketch:


http://www.forumimagecodes.com/image...tu4dkoiwdw.jpg
I would like to have a mesh of the blue part of the impeller: a single channel. I am using the periodicity tool of icem and the program is obviously not seeing that the vanes are rotating. I end up with a mesh which I can not use: the red part.

Is there any way I can mesh the single channel with an unstructured grid ?

thank you very muc

Will Anderson February 24, 2011 10:31

Meshing the single channel with an unstructured mesh is no problem. I did it by isolating the interior faces of the rotor blades, creating a separation line which runs down the middle of a rotor blade and continues in to the rotation axis and out to the exterior of the flow channel, extrude that line along the rotation axis into a face, copy and rotate that face about the rotation axis to the other rotor enclosing the channel, patching up the faces, and your channel is made.

I found difficulties downstream, in that I had a 2 stage radial compressor, and each stage had different periodicity, the inlet stator was meshed complete (360deg), the first rotor had 20deg periodicity, the second stator had 180deg periodicity, and this anarchy led to me not being able to force fluent to direct only an 18th of the massflow into stage1's rotor, for example. It may be easier to directly make a complete mesh, no periodicity, in order to ease computation and interpretation later on.

Quote:

Originally Posted by Mitpostdoc (Post 296609)
Thanks for the fast reply ;). Please, look at the following sketch:


http://www.forumimagecodes.com/image...tu4dkoiwdw.jpg
I would like to have a mesh of the blue part of the impeller: a single channel. I am using the periodicity tool of icem and the program is obviously not seeing that the vanes are rotating. I end up with a mesh which I can not use: the red part.

Is there any way I can mesh the single channel with an unstructured grid ?

thank you very muc


Mitpostdoc February 24, 2011 11:03

Thank you very much for the reply. If I understand the answer correctly you are saying to create a water tight geometry with surfaces which define the periodic boundaries and use the automatic unstructured mesh creator on it.

I though of that but I did not want to do it in the first place. The problem is that I will have to do the same for the impeller labyrinth seal which has a very very very complex geometry :(. If I will have to manually create lines and surfaces for it I will probably spend 4-5 day only fixing the gaps.

I guess that there is no other solution. I just hoped that Ansys had some automaic feature to grid turbomachinery without having to isolate manually the single passage.

Cheers!

PSYMN February 24, 2011 13:09

Right, if you give it the full geometry and just tell it an angle, how could you expect it to know that you want it to follow a curved shape. If you segment your geometry to match that periodic angle, then you are giving it both the angle and the shape and it should be fine...

Keep in mind that ICEM CFD is very tolerant of small faults and imperfections... You could split out this segment and mesh it without as much work fixing gaps as you are fearing...

Optionally, you could do this for the impeller and then copy rotate the mesh and do the seal in full.

PSYMN February 24, 2011 13:15

Another thought.
 
Actually, one more thought... It may be that you don't actually need to trim away the geometry, all you need to do is contain the mesh...

You could probably get away with just creating walls (one curves extruded thru the geometry) that follow that periodic shape and extend thru your model without cutting it... But you should create intersection curves between these surfaces and your model (so the mesh edge will be crisp). Then put a material point in the middle of the sector and mesh.

There is some wasted time as it will also mesh the rest of the model before throwing that portion away, but I think it will look after your periodicity on just the sector between the curved boundaries with the material point.

You could cut down on the wasted time by deleting surfaces outside your sector. The point is that it doesn't need to be a clean cut, and you don't actually need to trim any of the surfaces.

Mitpostdoc February 24, 2011 18:47

Quote:

Originally Posted by PSYMN (Post 296790)
Right, if you give it the full geometry and just tell it an angle, how could you expect it to know that you want it to follow a curved shape. If you segment your geometry to match that periodic angle, then you are giving it both the angle and the shape and it should be fine...

Keep in mind that ICEM CFD is very tolerant of small faults and imperfections... You could split out this segment and mesh it without as much work fixing gaps as you are fearing...

Optionally, you could do this for the impeller and then copy rotate the mesh and do the seal in full.

Thank you very much for the answer.:)
I hoped that since I have a shrouded impeller (closed impeller channels) Icem would have undestood the geometry and slimply followed the closed boundaries. Instead it is jumping from one sealed channel to the other forcing the continuity in between. My mistake.

I am sorry, I am not really confident with unstructured meshing in Icem.:p
I must be making some serious mistakes because I do not find Icem tolerant at all:(. I have performed several topology checks and looked around the geometry for holes everywhere.... the geometry seems water tight but Icem is still flooding of tetras the parts of the geometry which should be empty.

PSYMN February 25, 2011 11:51

Material Point...
 
Are you using material points?

If you don't put in material points, it assumes that all regions are of value. It will mesh each closed region with a different material.

In other words, are you sure it is leaking everywhere (same volume part in all regions), or is it just meshing everywhere (different volume part in each region)?


All times are GMT -4. The time now is 23:46.