CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

[ICEM] Meshing a centrifugal compressor impeller

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By Mitpostdoc

Reply
 
LinkBack Thread Tools Display Modes
Old   February 23, 2011, 12:57
Default [ICEM] Meshing a centrifugal compressor impeller
  #1
New Member
 
Claudio
Join Date: Feb 2011
Posts: 20
Rep Power: 6
Mitpostdoc is on a distinguished road
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?

I hope I have been clear enough, and I thank you for your help!
Mitpostdoc is offline   Reply With Quote

Old   February 23, 2011, 13:51
Default
  #2
Member
 
W.N. Anderson
Join Date: Jul 2010
Location: Zürich, Switzerland
Posts: 46
Rep Power: 7
Will Anderson is on a distinguished road
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.
Will Anderson is offline   Reply With Quote

Old   February 23, 2011, 16:30
Default
  #3
New Member
 
Claudio
Join Date: Feb 2011
Posts: 20
Rep Power: 6
Mitpostdoc is on a distinguished road
Thanks for the fast reply . Please, look at the following sketch:



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 is offline   Reply With Quote

Old   February 24, 2011, 10:31
Default
  #4
Member
 
W.N. Anderson
Join Date: Jul 2010
Location: Zürich, Switzerland
Posts: 46
Rep Power: 7
Will Anderson is on a distinguished road
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 View Post
Thanks for the fast reply . Please, look at the following sketch:



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 is offline   Reply With Quote

Old   February 24, 2011, 11:03
Default
  #5
New Member
 
Claudio
Join Date: Feb 2011
Posts: 20
Rep Power: 6
Mitpostdoc is on a distinguished road
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!
mina likes this.
Mitpostdoc is offline   Reply With Quote

Old   February 24, 2011, 13:09
Default
  #6
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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 is offline   Reply With Quote

Old   February 24, 2011, 13:15
Default Another thought.
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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.
PSYMN is offline   Reply With Quote

Old   February 24, 2011, 18:47
Default
  #8
New Member
 
Claudio
Join Date: Feb 2011
Posts: 20
Rep Power: 6
Mitpostdoc is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
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.
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.
Mitpostdoc is offline   Reply With Quote

Old   February 25, 2011, 11:51
Default Material Point...
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 36
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
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)?
PSYMN is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Meshing Error with a Solidworks Geometry Fractal ANSYS Meshing & Geometry 0 September 30, 2010 10:20
Basic steps meshing an airfoil [ICEM] peterputer111 ANSYS Meshing & Geometry 4 April 19, 2010 12:08
meshing blade centrifugal pump mino CFX 5 December 2, 2006 01:54
Singularity of grid?Volume meshing vs face meshing Ken Main CFD Forum 0 September 4, 2003 11:09
Volume Meshing & Face Meshing? singularity of grid ken FLUENT 0 September 4, 2003 11:08


All times are GMT -4. The time now is 13:32.