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

[ICEM] Icem cfd aerofoil meshing

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

Like Tree3Likes
  • 1 Post By diamondx
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   February 2, 2012, 13:04
Default Icem cfd aerofoil meshing
  #1
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 420
Rep Power: 12
cfd seeker is on a distinguished road
Hi all, I am facing problem in generating Unstructured Mesh of the aerofoil. After setting the parameters in "Part Mesh Setup" when i compute mesh on the surface, mesh goes through the aerofoil also. Kindly guide me through the proper steps for generating unstructured mesh on the aerofoil with prism layers and also having a density box.
Thanks in advance
cfd seeker is offline   Reply With Quote

Old   February 3, 2012, 11:12
Default
  #2
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 420
Rep Power: 12
cfd seeker is on a distinguished road
any body who know about this, kindly reply here as I am really stuck up in this problem.
cfd seeker is offline   Reply With Quote

Old   February 4, 2012, 16:10
Default
  #3
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Does mesh go "thru" the airfoil as if there is no boundary, or does the mesh go up to the airfoil and then there is also mesh inside the airfoil?

If the mesh is going thru the airfoil, then perhaps the curve is not part of the loop... Build topology to cut the surface with the curves.

If you just mean it is meshing inside the airfoil (as well as outside), then you have a decision... Do you want to model the solid (say for Conjugate heat transfer)? If not, then just delete the surface inside the airfoil. If yes, then just make sure that the surface inside is in a separate part so that you can apply solid properties to it...
__________________
-----------------------------------------
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   February 6, 2012, 09:55
Default
  #4
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 420
Rep Power: 12
cfd seeker is on a distinguished road
Thanks for replying Simon. Actually there is a mesh inside the aerofoil and I have to analyze the aerofoil to find the aerodynamic coefficients, so in this case mesh inside the aerofoil is not required. I am new to ICEM and I am totally unaware of geometry(topology). In the present case I have two curves representing the upper and lower sides of aerofoil and large circle representing the Farfield around the aerofoil. I tried to build a surface using the curves of Farfield and Aerofoil but the created surface is also passing inside the aerofoil, so mesh is also formed inside aerofoil. Kindly guide me how to create a surface which forms outside the aerofoil and how to give Size function, create prism layers in 2D?
I know about the quad-meshing tutorials but I am interested in the Unstructured(tri mesh) mesh for my case. Thanks in advance and waiting for your reply.
cfd seeker is offline   Reply With Quote

Old   February 6, 2012, 11:20
Default
  #5
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Just create a surface from the circle... It will pass thru the airfoil. You can put the surface in a new Part, perhaps named "FLUID".

Then Geometry (tab) => Geometry Repair => Build Diagnostic Topology. This will trim the surface with the airfoil curves and probably turn them red. You can then delete the surface within the airfoil.

For the unstructured patch conforming tri mesh you will need to set sizes on the curves. (under the mesh tab). When you set the sizes on the airfoil, you can set a number of layers, initial height and growth ratio...

Then surface mesh with patch conforming and you should be done (with boundary layers).

If you want a fancier boundary layer using the actual prism executable, you will need to turn on the advanced option for blayer2d. Search CFD online for that and I am sure you will find lots of posts...

If I were meshing this airfoil in a circle, I would use ICEM CFD Hexa. You can find a video about how to do that here... http://www.youtube.com/watch?v=tYrbS...3&feature=plcp
__________________
-----------------------------------------
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   February 7, 2012, 15:34
Default
  #6
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,366
Blog Entries: 23
Rep Power: 21
diamondx will become famous soon enough
I'm new to ICEM too, but i hope that you might find it useful.
[URL="http://www.youtube.com/watch?v=tYrbScUH9RE"]
The guy creates a mesh around aerofoil...
cheers,
ALI
PSYMN likes this.
diamondx is offline   Reply With Quote

Old   February 7, 2012, 15:37
Default
  #7
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,285
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
The name of that guy is PSYMN
BrolY likes this.
Far is offline   Reply With Quote

Old   February 7, 2012, 15:41
Default
  #8
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,366
Blog Entries: 23
Rep Power: 21
diamondx will become famous soon enough
the guy's name "Simon Pereira"
diamondx is offline   Reply With Quote

Old   February 8, 2012, 04:51
Default
  #9
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 420
Rep Power: 12
cfd seeker is on a distinguished road
@Simon
your guidance help me a lot,thanks a lot. I have manged to have a surface outside aerofoil and also able to mesh it,I have also applied the prism layers but prism near the trailing edge is not respecting the geometry of aerofoil rather it is passing inside it, I have also increased the no. of nodes on the aerofoil curves but all in vein, so kindly tell me how to tackle this problem? Secondly I am interested in applying a density region on the upper surafce of aerofoil to capture the separation at higher angle of attacks but the mesh is not taking that density region into consideration( mesh forms as without the density box), what's the problem here? what mistake I am making in applying density box. I have build the density box using the four created points other than the aerofoil.
cfd seeker is offline   Reply With Quote

Old   February 8, 2012, 21:39
Default
  #10
Retired from CFD Online
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
The density box only works with the octree or delaunay tetra meshers...

MultiZone does not respect it (yet).

Not sure about your other issue... Maybe a picture...
__________________
-----------------------------------------
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

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
Learn ANSYS ICEM CFD easy_astronaut ANSYS 2 December 15, 2013 16:34
definition of "node" / "element" in CFX and ICEM CFD murx CFX 3 May 29, 2011 12:08
[ICEM] Some meshing quieries with ICEM CFD saisanthoshm88 ANSYS Meshing & Geometry 11 April 22, 2011 12:19
ICEM CFD use for ? Vu Trinh Tuan CFX 14 April 11, 2011 18:38
ICEM CFD Modules Boris FLUENT 1 March 12, 2004 15:37


All times are GMT -4. The time now is 06:01.