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

[ICEM] Mesh unable to follow curved geometry

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

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 5, 2012, 04:47
Default Mesh unable to follow curved geometry
  #1
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
Hi..
I am trying to mesh a wing with sinusoidal leading edge..
My problem is that the mesh does not follow the profile of the leading edge UNLESS i give very high bunching as seen near the tip of the wing below..

As you move towards the root of the wing, the mesh is less concentrated and it does not follow the profile..

I need a way to make the mesh follow the profile inspite of lesser number of nodes( currently the node spacing near the root is 0.002 and if i have such spacing throughout the span, total elements become more than 10 million which is not reasonable for me..)

https://dl.dropbox.com/u/79881940/files.rar

The above link contains the block and tin files

thanks....


Last edited by Ananthakrishnan; June 5, 2012 at 05:49.
Ananthakrishnan is offline   Reply With Quote

Old   June 5, 2012, 05:03
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
try option project to b-spline.
Far is offline   Reply With Quote

Old   June 5, 2012, 05:19
Default
  #3
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
i tried it and i dont see any changes ( ..
let me upload the .blk and .tin files..
Ananthakrishnan is offline   Reply With Quote

Old   June 5, 2012, 05:37
Default
  #4
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
https://dl.dropbox.com/u/79881940/files.rar

the block and tetin files are available in the above URL..

@far..To use project to b spline option, i just need to select it and "apply" right?? after this if i recompute the pre mesh i dont see any changes...
Ananthakrishnan is offline   Reply With Quote

Old   June 6, 2012, 14:52
Default
  #5
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
It is clear that your mesh size along the wing is larger than the features you are trying to capture... You will need much finer mesh (increase the number of nodes) along the wing...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   June 7, 2012, 02:17
Default
  #6
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
If i try to capture the features by just increasing the nodes, then the mesh size increases drastically (around 8 million). It is practicably not feasible for me at all..
Is there any other way to do it??
Ananthakrishnan is offline   Reply With Quote

Old   June 7, 2012, 13:57
Default
  #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
You may be able to increase the resolution in that area without increasing everywhere (either with clever topology, or with refined blocks (hanging nodes), sub models, or other methods), but you can't expect to capture that trailing edge with mesh that is coarser than the edge...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   June 9, 2012, 06:48
Default
  #8
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
Thanks a lot..i was able to create the hanging nodes by mesh refinement but the nodes are not getting projected onto the curves..
I have switched on the "project to B splines" option as well..any ideas??

Ananthakrishnan is offline   Reply With Quote

Old   June 11, 2012, 15:09
Default
  #9
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
hello ananthakrishnan,



did you consider a mix of hexa and tri. i tried and ended up with 3M node like the picture above. may be you will need a more refined mesh depending on you flow around the wing.
I attached the project, file size is 150 Mb because of the *.*uns file. What is your computer specs ? can you handle opening 5M-6M. let me know if you can, then you can set up a case file, then share it with me, i can help you perform calculation on a cluster (big cluster i have access to).

the project file: https://dl.dropbox.com/u/35161486/Ananthakrishnan.zip
hadikhayyamian likes this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 11, 2012, 15:10
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
how did u make the hybrid meshing?
Far is offline   Reply With Quote

Old   June 11, 2012, 15:15
Default
  #11
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
i made a small box around the airfoil, i named all the surfaces of the box "interface". then i meshed inside of the box using blocking and outside of the box with unstructured and giving a very small size to the tri element next to hexa so the merging process can be done well, after that i went to mesh and merged the two of them and selected "interface" as the common part.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 11, 2012, 15:19
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
both meshes need to be identical at interface? If yes, how to ensure this?
Far is offline   Reply With Quote

Old   June 11, 2012, 15:29
Default
  #13
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
yes they have to be identical, regarding what ? size, i use the measure distance to calculate length of a hexa element. then i copy that length in the tri size.
That's the only way i found and the only way i know for merging two meshes. Then i trust the program in the merging process to do the adequate change in size and merging the node .
Please let me know of another trustful way.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 12, 2012, 02:35
Default wavy wall
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
See this type of topology advance toplogy , Refer to Fig. no. 5d and 5e. Although it is different software, but still you can idea how to proceed without increasing the mesh size.
Far is offline   Reply With Quote

Old   June 12, 2012, 03:26
Default
  #15
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
@diamondx
thats awesome..sorry i was not able to reply immediately (damn exams)...Thnaks for the cluster man...seriously...let me put my comp to acid test first...
tried the hybrid mesh but wasnt sure about the merging at the interface..i ended up having two sets of nodes at the interface one each for structured and unstructured(even though the size was matching)

i am thinking about "merge sheet with block" option...

Last edited by Ananthakrishnan; June 12, 2012 at 03:57.
Ananthakrishnan is offline   Reply With Quote

Old   June 12, 2012, 04:23
Default
  #16
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,969
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
delete line elements at interface (as suggested by Simon as I remember)
Ananthakrishnan likes this.
Far is offline   Reply With Quote

Old   June 14, 2012, 05:58
Default
  #17
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
Thanks to all i was able to get a decent mesh..But as of now i am unable to merge the two meshes.

What option should i use in "merge nodes" for merging the two meshes.
I initially thought if i create the unstructured mesh by using the existing mesh on the surface of the interface, then the two meshes are automatically merged!!!

https://www.dropbox.com/s/nu3y4ekrll...%20flipper.rar

Last edited by Ananthakrishnan; June 14, 2012 at 07:27.
Ananthakrishnan is offline   Reply With Quote

Old   June 14, 2012, 14:20
Default
  #18
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
are you using icem 14 ? can't open your project
in merge nodes, select merge meshes, leave the default setting and select the surface that the tri and the hexa has in common in the "merge surface mesh parts"
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 14, 2012, 14:40
Default
  #19
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
ok no it's version 13. but when i open the project everything disappear. can you open it and dismiss the scan plane operation then save it again ? thanks
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   June 14, 2012, 15:01
Default
  #20
Senior Member
 
Ananthakrishnan.A.S
Join Date: Feb 2012
Location: Mumbai (Bombay), India
Posts: 146
Rep Power: 7
Ananthakrishnan is on a distinguished road
Send a message via Skype™ to Ananthakrishnan
done..It should be working now

Last edited by Ananthakrishnan; June 14, 2012 at 16:07.
Ananthakrishnan is offline   Reply With Quote

Reply

Tags
curved edge, interface, merge mesh, mesh control, sinusoidal leading edges

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
Irregular mesh generation for simple box geometry ajl42 OpenFOAM Native Meshers: snappyHexMesh and Others 0 March 7, 2011 18:04
Need help with the error cfdproject OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 0 April 14, 2009 15:45
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
vitual _ real deneb FLUENT 3 January 22, 2007 05:31
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 17:00.