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

[ICEM] unknown pre-mesh distortion

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

Like Tree3Likes
  • 2 Post By cesarcg
  • 1 Post By diamondx

Reply
 
LinkBack Thread Tools Display Modes
Old   July 14, 2013, 22:49
Default unknown pre-mesh distortion
  #1
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
Dear veteran meshers,

After long and repeated meshing work ,i got quite a frustrated results:the mesh over one side of the aircraft is mysteriously distorted ,while the opposite side is fine.The two sides are symmetrical.
I did the association work for curves and faces all over again,but the results are the same.Can you help locate the problem of this issue,I really don't want to redo the blocking and splitting....
Attached Images
File Type: jpg 1.jpg (100.7 KB, 26 views)
File Type: jpg 2.jpg (100.3 KB, 27 views)
File Type: jpg 3.jpg (99.9 KB, 21 views)
treenw is offline   Reply With Quote

Old   July 15, 2013, 02:30
Default
  #2
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
problem solved after re-create the nacelle geometry.
treenw is offline   Reply With Quote

Old   July 15, 2013, 03:29
Default
  #3
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
you are making full hexa?
Far is offline   Reply With Quote

Old   July 15, 2013, 07:52
Default
  #4
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
Quote:
Originally Posted by Far View Post
you are making full hexa?
yes,FAR.quite stupid I know ,very grid-inefficient,already got 600 million,barely run on my 16G RAM PC.
Just want to see the whole picture.
Still got the Y-block generated mesh around the dorsal fin with ANGLE critiria like shit ,any suggestions?
Attached Images
File Type: jpg 4.jpg (99.5 KB, 16 views)
treenw is offline   Reply With Quote

Old   July 15, 2013, 11:39
Default
  #5
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
the procedure is time consuming !!! expect bad element quality if you don't simply geometry. you should add o-grid for the engine's nozzle exit...
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   July 15, 2013, 12:13
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by treenw View Post
yes,FAR.quite stupid I know ,very grid-inefficient,already got 600 million,barely run on my 16G RAM PC.
Just want to see the whole picture.
Still got the Y-block generated mesh around the dorsal fin with ANGLE critiria like shit ,any suggestions?
It will take some time. Look at the meshes by Simon done for drag prediction workshop
Far is offline   Reply With Quote

Old   July 15, 2013, 15:55
Default
  #7
Member
 
Cesar
Join Date: Nov 2012
Location: Guanajuato, México
Posts: 78
Rep Power: 6
cesarcg is on a distinguished road
Send a message via Skype™ to cesarcg
Quote:
Originally Posted by treenw View Post
yes,FAR.quite stupid I know ,very grid-inefficient,already got 600 million,barely run on my 16G RAM PC.
Just want to see the whole picture.
Still got the Y-block generated mesh around the dorsal fin with ANGLE critiria like shit ,any suggestions?
Why are those cells so distorted? Won't you use the symmetry boundary condition to reduce the number of cells? I think that the Y-block may be not necessary.

Regards.
cesarcg is offline   Reply With Quote

Old   July 16, 2013, 22:56
Default
  #8
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
Quote:
Originally Posted by diamondx View Post
the procedure is time consuming !!! expect bad element quality if you don't simply geometry. you should add o-grid for the engine's nozzle exit...
Hi diamandx,
Thanks for reply,how do you think i should simplify the geometry,for me it's already the basic aerodynamic shape of a aircraft.
And the engine exhaust blocks are already splitted like this:
Attached Images
File Type: jpg 4.jpg (94.9 KB, 11 views)
File Type: jpg 5.jpg (96.5 KB, 15 views)
treenw is offline   Reply With Quote

Old   July 16, 2013, 23:12
Default
  #9
Member
 
Cesar
Join Date: Nov 2012
Location: Guanajuato, México
Posts: 78
Rep Power: 6
cesarcg is on a distinguished road
Send a message via Skype™ to cesarcg
I suggest you to use a symmetry boundary condition in order to reduce the number of cells and to simplify the blocking procedure. Otherwise you will require a huge quantity of memory to be able to load the mesh into fluent or any other CFD code. I also see that you have a Y-block right behind the exhaust of the nozzle, which in my particular point of view is adding unnecessary complexity to the blocking topology.

I guess that diamondx is suggesting to implement an o-grid topology at the face of the exhaust like the one shown in the attached picture. That would help to avoid significantly those distorted cells you have in your recent mesh.

http://laurent.nack.pagesperso-orang...cem/grido1.gif

Regards,
César
diamondx and treenw like this.
cesarcg is offline   Reply With Quote

Old   July 16, 2013, 23:25
Default
  #10
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
Another thing, you could have used symmetry for your geometry and then transforming that mesh by mirroring it...
@FAR, have you got any geometry like this, this can be a good subject for a contest...
Far likes this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   July 17, 2013, 21:48
Default
  #11
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
Quote:
Originally Posted by Far View Post
It will take some time. Look at the meshes by Simon done for drag prediction workshop
great tip!
I'm right now learning the stuff from drag prediction workshop searched from google.
thanks!
treenw is offline   Reply With Quote

Old   July 17, 2013, 21:57
Default
  #12
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
Quote:
Originally Posted by cesarcg View Post
Why are those cells so distorted? Won't you use the symmetry boundary condition to reduce the number of cells? I think that the Y-block may be not necessary.

Regards.
HI Cesarcg,
those cells are distorted due to some geometry association promblem,already smoothed after re-create part.
Didn't use the split-in-half model because i really want to see the unsymmetrical flow pattern expected for later purposes.
And for Y-block,i just don't know any other methods to split a sharp edge wing tip block.
treenw is offline   Reply With Quote

Old   July 17, 2013, 22:02
Default
  #13
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
Quote:
Originally Posted by diamondx View Post
Another thing, you could have used symmetry for your geometry and then transforming that mesh by mirroring it...
@FAR, have you got any geometry like this, this can be a good subject for a contest...
good idea,that should save half the trouble i expect.
treenw is offline   Reply With Quote

Old   July 17, 2013, 22:30
Default
  #14
New Member
 
Join Date: May 2013
Posts: 8
Rep Power: 4
treenw is on a distinguished road
Quote:
Originally Posted by cesarcg View Post
I suggest you to use a symmetry boundary condition in order to reduce the number of cells and to simplify the blocking procedure. Otherwise you will require a huge quantity of memory to be able to load the mesh into fluent or any other CFD code. I also see that you have a Y-block right behind the exhaust of the nozzle, which in my particular point of view is adding unnecessary complexity to the blocking topology.

I guess that diamondx is suggesting to implement an o-grid topology at the face of the exhaust like the one shown in the attached picture. That would help to avoid significantly those distorted cells you have in your recent mesh.

http://laurent.nack.pagesperso-orang...cem/grido1.gif

Regards,
César

Thank you Cesar,very good suggestion,much appreciated.

That o-grid should eliminate the low quality cells at the end of cylinder-shaped nacelles and fuselage,I suppose?

Also I didn't use symmetry boundary because i had unrealistic confidence of my 8-core 16G ram PC(I used to have a Pentium 4 with 2G ram that can handle 1 million grids),infact 600 million is alomost the limit for now,with first-order and turbulence on.I'll resort to half model if this full hexa approach dosen't work out.

Please shine some light on the blocking strategy for my four sharp edge parts without using Y-block:wings,horizental tail,nacelles,dorsal fin(pointed at the frontmost) .
Attached Images
File Type: jpg 6.jpg (98.8 KB, 13 views)
treenw is offline   Reply With Quote

Old   July 19, 2013, 01:28
Default
  #15
Member
 
Cesar
Join Date: Nov 2012
Location: Guanajuato, México
Posts: 78
Rep Power: 6
cesarcg is on a distinguished road
Send a message via Skype™ to cesarcg
Quote:
Originally Posted by treenw View Post
Thank you Cesar,very good suggestion,much appreciated.

That o-grid should eliminate the low quality cells at the end of cylinder-shaped nacelles and fuselage,I suppose?
Yes, I think that should improve the quality of the cells. It is very important to avoid cells with very acute angles. Read this post by Far for further inquiries Mesh quality criteria

Quote:
Also I didn't use symmetry boundary because i had unrealistic confidence of my 8-core 16G ram PC(I used to have a Pentium 4 with 2G ram that can handle 1 million grids),infact 600 million is alomost the limit for now,with first-order and turbulence on.I'll resort to half model if this full hexa approach dosen't work out.
I don't know what you mean with having unrealistic confidence of your 8-core PC. First of all, what type of numerical analysis are you pretending to do? I mean, do you want to focus on specific parts of the geometry of the aircraft? If so, that will be helpful to give more importance to the nacelles, or wings, or fuselage, etc.

Quote:
Please shine some light on the blocking strategy for my four sharp edge parts without using Y-block:wings,horizental tail,nacelles,dorsal fin(pointed at the frontmost).
The meshing of the rear part of the aircraft will be very time consuming, if successful, lol. Maybe, you'll have to start thinking how to simplify the geometry as suggested by diamondx, since in my short experience the region where the engine is joined to the fuselage, by means of an extruded-airfoil-like geometry, will be very difficult to mesh. This last assuming that you try to mesh it with hexa.

Regards.
cesarcg 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
Star CCM Overset Mesh Error (Rotating Turbine) thezack CD-adapco 3 December 11, 2013 04:09
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Mesh distortion close to cylind wall-GAMBIT 2.2.30 Mirek FLUENT 1 April 15, 2006 17:22
How to control Minximum mesh space? hung FLUENT 7 April 18, 2005 09:38


All times are GMT -4. The time now is 07:15.