CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

TG mesh density

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 10, 2016, 02:23
Default TG mesh density
  #1
Member
 
Alex
Join Date: Feb 2016
Posts: 50
Rep Power: 2
Red Ember is on a distinguished road
I generated mesh for several compressor stages using turbogrid. Looking at borders between stages (e.g. - first stage and second stage) it's obvious that mesh density differs. Are there any suggestions for volume/length ratios for cells that belong to different domains? I use GGI interface option in CFX-PRE, but I think that's not enough...
Attached Images
File Type: jpg Different mesh density.jpg (174.8 KB, 26 views)
Red Ember is offline   Reply With Quote

Old   February 10, 2016, 06:48
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I would go back to turbogrid and try to make the mesh size more even. That does not look good to me.

To prove whether it is a problem or not - do a simulation on this mesh and then significantly change the mesh and repeat it. If the results are significantly different then you know the mesh change you did is significant - which probably means the mesh quality at the interfaces is not adequate.
ghorrocks is offline   Reply With Quote

Old   February 10, 2016, 10:14
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 115
Rep Power: 9
turbo is on a distinguished road
Increase grid numbers in both inlet and outlet domains in TG.

You will see the function allows only a uniform spacing there, which is so frustrating. I had argued with Ansys support on this issue, and they said they would submit a request to improve it. I doubt they will do. That's what CFX is now.
turbo is offline   Reply With Quote

Old   February 11, 2016, 02:13
Default
  #4
Member
 
Alex
Join Date: Feb 2016
Posts: 50
Rep Power: 2
Red Ember is on a distinguished road
ghorrocks,
yes, I tried to make elements at borders more equal, although it caused some increase of nodes number. I'll try to compare results.

turbo,
I used "increase edge refinement" function for local mesh density smoothing. Number of elements at inlet/outlet is linked to number at blade surface, so it's not easy to create mesh without local high concentration of elements. Moreover, I see no way to open all domains using TG, I compare grids using postprocesor. Rather annoying too...
Red Ember is offline   Reply With Quote

Old   February 12, 2016, 01:16
Default
  #5
Member
 
Alex
Join Date: Feb 2016
Posts: 50
Rep Power: 2
Red Ember is on a distinguished road
My refinements yielded no significant differences.
Too bad, I thought mesh was a reason why calculated compressor efficiency value is very low - about 60%...
Red Ember is offline   Reply With Quote

Old   February 12, 2016, 09:52
Default
  #6
Senior Member
 
Maxim
Join Date: Aug 2015
Location: Germany
Posts: 304
Rep Power: 4
-Maxim- is on a distinguished road
in order to get a 'nicer' mesh around the blades, you could try another topology in TG. Activate advanced/beta features to get more options.
I usually work with edge refinements as well, so that sounds good to me.

Maybe post in the meshing subforum in case you would like more improvements there.
Otherwise you might share and discuss the rest of your project so that we could try to help to find out why you don't get your expected compressor efficiency.

edit: just saw your other post about the compressor efficiency

Last edited by -Maxim-; February 12, 2016 at 09:53. Reason: saw other post
-Maxim- is offline   Reply With Quote

Old   February 12, 2016, 11:08
Talking
  #7
Senior Member
 
Join Date: Jun 2009
Posts: 115
Rep Power: 9
turbo is on a distinguished road
Quote:
Originally Posted by Red Ember View Post
My refinements yielded no significant differences.
Too bad, I thought mesh was a reason why calculated compressor efficiency value is very low - about 60%...
Because your blade design was wrong, not the mesh.
turbo is offline   Reply With Quote

Old   February 12, 2016, 14:29
Default
  #8
Member
 
Alex
Join Date: Feb 2016
Posts: 50
Rep Power: 2
Red Ember is on a distinguished road
-Maxim-,
actually I don't blame mesh now, mesh was fine within every domain. Then I made cell sizes near domain interfaces more equal, so that's enoufg for now. I just wonder whether exist any ratio criteria for elements that belong to different domains but have common border or not.

turbo,
I made several assumptions that increase numerical errors.
1. I have no geometry for the last, 7th stage, so I simulate only 6 stages (plus inlet guide vanes). I get outlet pressure via interpolation (not proper accurate, but better than nothing). I use outlet flow direction normal to outlet surface for now. I'll estimate approximate angle value a bit later.
2. I used merge operation to get one flowpath sketch for 6 stages at once. That distorted hub surface:
http://www.cfd-online.com/Forums/ans...istortion.html
I think I should chop this sketch in 13 parts to improve hub line, although I suspect somewhat problems with domain interfaces geometry can pop out.
3. Shroud tips and hub tips - not all of them can be simulated via turbogrid tip options (or may be I just am not aware of it). Tip span and absolute values are not constant! Tip and hub/shroud curves are not equidistant in my case. So I had to accept normal distance tip option.
4. I faced problems with curves around fillets. No exportpoints were created. I'll try to create more curves around fillets.
5. Inlet guide vanes and first stage guide vanes are variable. So there are dashed hub and shroud tips that I can't simulate using TG.

But blades and vanes design is good enough due to static pressure contours.
Red Ember is offline   Reply With Quote

Old   February 15, 2016, 22:56
Default
  #9
Senior Member
 
Join Date: Jun 2009
Posts: 115
Rep Power: 9
turbo is on a distinguished road
I assume your task is to simulate an existing 7-stage axial compressor in CFX by importing blade solids from CAD. What you did is not a recommended procedure. You need to build a BladeGen model of each blade row from xyz surface coordinates from CAD. You have to visit BG 15 times for your case. Then TG > CFX.
turbo is offline   Reply With Quote

Old   February 17, 2016, 14:42
Default
  #10
Member
 
Alex
Join Date: Feb 2016
Posts: 50
Rep Power: 2
Red Ember is on a distinguished road
turbo, thanks for advice!
Yep, existing compressor. But why it is not recommended? That's definitely new for me, can you give me reason why? Or share a link, please! I'd like to read smth about it.
So! If I get you right, I should use BG instead of Design Modeler and Blade Modeler preference?
Red Ember is offline   Reply With Quote

Old   February 17, 2016, 17:14
Default
  #11
Senior Member
 
Join Date: Jun 2009
Posts: 115
Rep Power: 9
turbo is on a distinguished road
That is why You made such many assumptions in the geometry including flowpath curves. If you split each row to model in BG, you can minimize any mismatch with the real blades.
turbo is offline   Reply With Quote

Old   February 17, 2016, 23:44
Default
  #12
Member
 
Alex
Join Date: Feb 2016
Posts: 50
Rep Power: 2
Red Ember is on a distinguished road
turbo, is TG able to reproduce fillets and non-trivial curvature at end clearance if I use BladeGen before TurboGrid? And how I should get coords for BladeGen - import 3D models or get coords in CAD soft at first and then use it in BladeGen?
Red Ember is offline   Reply With Quote

Old   February 18, 2016, 14:45
Default
  #13
Senior Member
 
Join Date: Jun 2009
Posts: 115
Rep Power: 9
turbo is on a distinguished road
If you want blade fillets and/or custom tip clearance, BG > DM > TG > CFX
turbo is offline   Reply With Quote

Old   February 18, 2016, 23:45
Default
  #14
Member
 
Alex
Join Date: Feb 2016
Posts: 50
Rep Power: 2
Red Ember is on a distinguished road
And what about coords?
Red Ember is offline   Reply With Quote

Old   February 20, 2016, 10:04
Default
  #15
Senior Member
 
Join Date: Jun 2009
Posts: 115
Rep Power: 9
turbo is on a distinguished road
Get all xyz surface coordinates at spanwise sections > BGD model > Fillets in DM > Export to TG > CFX
turbo 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
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
[ICEM] Using mesh Density Daniel_Khazaei ANSYS Meshing & Geometry 0 May 2, 2014 18:00
Mesh motion with Translation & Rotation Doginal CFX 2 January 12, 2014 07:21
Layers:problem with curvature giulio.topazio OpenFOAM Native Meshers: snappyHexMesh and Others 10 August 22, 2012 09:03
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11


All times are GMT -4. The time now is 19:40.