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

[ICEM] Boundary layer problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 6, 2011, 13:14
Default [ICEM] Boundary layer problem
  #1
New Member
 
Papis
Join Date: Dec 2010
Posts: 25
Rep Power: 6
papis is on a distinguished road
Hi,

I did an unstuctred mesh of a NACA 0012 with 20 layers.The thing is that it is very bad at the trailing edge and i don't know why.

The procedure i followed to create the mesh was :
  1. Imported airfoil geometry(2 curves)
  2. Create farfield points and surface
  3. Segmented farfield surface with the airfoil curves
  4. Deleted airfoil surface
  5. Defined curve mesh setup(layers/nodes)
  6. Adjusted model tolerance from 0.007 to 1e-07 (0.007 spoiled trailing edge geometry)
  7. Computed mesh
Any ideas what is the problem? I can't really get it

Screenshots
http://147.102.42.169/icem/unstr1.png
http://147.102.42.169/icem/unstr2.png
papis is offline   Reply With Quote

Old   June 7, 2011, 06:38
Default
  #2
New Member
 
Papis
Join Date: Dec 2010
Posts: 25
Rep Power: 6
papis is on a distinguished road
Fixed. I actually did it with multizone Hexa/Mixed blocking. the boundary layer is good.

Don't know why surface mesh fails.
papis is offline   Reply With Quote

Old   June 7, 2011, 10:15
Default Trailing edge curve...
  #3
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
A popular "trick" for unstructured mesh is to create a trailing edge curve behind the airfoil... This gives the prisms something to continue back with...

I have posted other images on CFD Online, but are a couple examples...
Attached Images
File Type: jpg CZ_03.jpg (107.7 KB, 98 views)
File Type: jpg Joel_8_BetterPrism.jpg (60.3 KB, 77 views)
__________________
-----------------------------------------
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, 2011, 12:22
Default
  #4
New Member
 
Papis
Join Date: Dec 2010
Posts: 25
Rep Power: 6
papis is on a distinguished road
Thank you very much for you help.

There is another issue I have questions

At the picture below is a multizone mesh. with free blocks.The edge mesh setup in the red circle is like 10e-04(spacing1) where as in the green circle is 10e-05.As you can see free blocks when 10e-05 spacing is used are not meshed.

I guess it's a tolerance issue,because when i make the edge spacing coarser everything is meshed.I know the grid isn't very good,but it's critical to understand the reason behind this issue.Not mater how small the model geometry tolerance is nothing changes. Is there an internal limit for how small unstructured mesh shells can be?

Thanks again for your time.

papis is offline   Reply With Quote

Old   June 7, 2011, 12:45
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: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Meshing a free block uses a recursive loop paving algorithm...

It starts from the line elements around the perimeter and paves inward... Along the way, it checks quality and can make adjustments to the paving in order to keep quality up...

In your case, with the size difference so huge between the horizontal and vertical edges, the elements created are such poor quality that the adjustments can't help and the loop fails to mesh.

When you adjust the sizes on that vertical edge so that the corner mesh is a little closer to matching (you can then have it grow away from that corner), the initial loop has a much better chance and you get a mesh in the loop...
__________________
-----------------------------------------
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, 2011, 15:34
Default
  #6
New Member
 
Papis
Join Date: Dec 2010
Posts: 25
Rep Power: 6
papis is on a distinguished road
You are SO right. Thank you very much for your help.
papis is offline   Reply With Quote

Old   October 23, 2013, 17:29
Default
  #7
New Member
 
Jason
Join Date: May 2013
Location: South Africa
Posts: 29
Rep Power: 4
jasonbot is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
A popular "trick" for unstructured mesh is to create a trailing edge curve behind the airfoil... This gives the prisms something to continue back with...

I have posted other images on CFD Online, but are a couple examples...
Can this trick be used for blunt trailing edges too?

I'm having a problem with mine when using patch conforming unstructured mesh setups.
Attached Images
File Type: jpg mesh problem.jpg (47.1 KB, 36 views)
jasonbot is offline   Reply With Quote

Old   October 23, 2013, 22:02
Default
  #8
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Quote:
Originally Posted by jasonbot View Post
Can this trick be used for blunt trailing edges too?

I'm having a problem with mine when using patch conforming unstructured mesh setups.
In your case, I would suggest setting a smaller size on the trailing edge and setting ortho weight to 0.5 so the prisms will lean into the corner (it looks like you have it set to 1.0)
__________________
-----------------------------------------
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   October 24, 2013, 02:09
Default
  #9
New Member
 
Jason
Join Date: May 2013
Location: South Africa
Posts: 29
Rep Power: 4
jasonbot is on a distinguished road
Quote:
Originally Posted by PSYMN View Post
In your case, I would suggest setting a smaller size on the trailing edge and setting ortho weight to 0.5 so the prisms will lean into the corner (it looks like you have it set to 1.0)
I suspect this is for a 2D prism mesh and not a shell mesh?
jasonbot is offline   Reply With Quote

Old   October 24, 2013, 15:50
Default
  #10
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Quote:
Originally Posted by jasonbot View Post
I suspect this is for a 2D prism mesh and not a shell mesh?
Oh yea, the shell mesh offset is really just designed for bolt holes (FEA), not 2D N-S flow...

Instead, try using "blayer2D" to generate higher quality boundary layers. There are a number of threads about that if you want more info.
__________________
-----------------------------------------
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   October 25, 2013, 06:53
Default
  #11
New Member
 
Jason
Join Date: May 2013
Location: South Africa
Posts: 29
Rep Power: 4
jasonbot is on a distinguished road
Quote:
Originally Posted by PSYMN
Oh yea, the shell mesh offset is really just designed for bolt holes (FEA), not 2D N-S flow...

Instead, try using "blayer2D" to generate higher quality boundary layers. There are a number of threads about that if you want more info.

***just a note: I am used to using ICEM for clean airfoils, by means of blocking. I am currently working on a high lift airfoil in which blocking has not been successful. Hence my need to learn the unstructured prism mesh tools***

I've tried following steps in the other threads
I have reverted back to the most basic of geometries, a domain with a circle in it. Just to try and get the hang of Prism meshing.

Here are my steps:

1. I created a square in ICEM and drew a circle inside.
2. Create surface from square edges.
3. Create 2D Planar block.
3. Associate square edges with surface edges.
4. Associate block with surface.
5. Use segment tool to cut out the circle where we need no flow.

6. Global mesh setup.
6.1 Volume mesh set up as tet/mixed, robust (octree) method.
6.2 Prism mesh set up as linear with three layers, advanced setting: blayer2d on.

7. Fluid region has prism setting ticked with height, ratio and num layers set.
7.1 apply inflation to curves ticked.

8. Compute mesh, volume mesh, create prism layers checked.

Compute gives me this...

I think I'm doing something wrong with the way I am handling my geometry?
Attached Images
File Type: png prismmesh1.png (24.8 KB, 22 views)
jasonbot 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
Boundary layer generation problems ivan_cozza OpenFOAM Native Meshers: snappyHexMesh and Others 0 October 6, 2010 13:47
Boundary Layer Question scottneh STAR-CCM+ 3 September 30, 2010 14:21
2D Boundary Layer Development in CFX11 Chris Basciano CFX 1 August 28, 2008 16:15
problem with boundary layer Bharath Main CFD Forum 1 July 11, 2008 09:06
GAMBIT meshing problem for boundary layer Falah FLUENT 1 October 9, 2006 03:32


All times are GMT -4. The time now is 22:45.