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

[ICEM] 3D mesh of airfoil from 2D

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

Like Tree2Likes
  • 1 Post By BrolY
  • 1 Post By TKE

Reply
 
LinkBack Thread Tools Display Modes
Old   October 5, 2011, 04:31
Smile 3D mesh of airfoil from 2D
  #1
TKE
New Member
 
TKE's Avatar
 
Jozsef Rideg
Join Date: Feb 2011
Location: Budapest, Hungary
Posts: 21
Rep Power: 6
TKE is on a distinguished road
Hi everyone,

I have the following problem: I have made a 2D mesh around an airfoil. I would like to generate a 3D one, I would like to extrude it in spanwise direction with a certain length and a certain number of cells, but with the same 2D structure. As I realized, there are two ways of making it:

1) EXTRUDE
a) Convert into unstructured mesh
b) Extrude mesh. (number of cell: x, size of cells: y)

My problem: the parts (AIRFOIL_SS, AIRFOIL_PS, IN, OUT, TOP_SYMMETRY, BOTTOM_SYMMETRY) are lines. I have a 3D mesh with line element parts.
I do not know, whether it is possible to define surfaces on an unstructured mesh?
How should I define the boundary conditions on surfaces if I have an unstructured 3D mesh?

2) 3D BLOCK
a) I copy all the parts and geometry entities (points, curves) in spanwise direction.
b) I connect the curves (for example original AIRFOIL_SS with the new, translated AIRFOIL_SS_01)
b) I define the necessary surfaces:
AIRFOIL_SS, AIRFOIL_PS, IN, OUT, TOP_SYMMETRY, BOTTOM_SYMMETRY, and 2 extra with spanwise normal vector: PERIODIC_1, PERIODIC_2 (for LES).

The problem: I have surfaces, the wire frame of the body, but I have only 2D block structure, which should be kept and transformed into 3D. But I do not know how to make it?
(creating 3D blocks, doing associations again? material points?)

Probably I would prefer the 1st version, because in that case at least I have the demanded mesh itself, and only the problem is that it is unstructured and I do not know how to define the surface boundary conditions on it, as it has only curves as defined parts.

Thank you for your hints!

Regards,
TKE
TKE is offline   Reply With Quote

Old   October 5, 2011, 05:17
Default
  #2
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
1) When you extrude your mesh, you have to choose the name for the new volume mesh, the new side mesh and the new top mesh. Check all the option of the extrude which can be nice (specify the number of nodes on the extude curve for example). Once the extrude is done, you can create parts by adding the shells created by the extrude to your new part. And then apply the boundary conditions on the created parts.

2) About the blocking : Blocking -> Create Block -> Extrude Face and choose extrude along a curve. But you have to create the geometry of the extrude before to associate the blocks to geometry. Then associate curves etc ...

The first option would be the fastest and easiest I think.
Have fun
TKE likes this.
BrolY is offline   Reply With Quote

Old   October 6, 2011, 05:44
Default Thanks
  #3
TKE
New Member
 
TKE's Avatar
 
Jozsef Rideg
Join Date: Feb 2011
Location: Budapest, Hungary
Posts: 21
Rep Power: 6
TKE is on a distinguished road
Thank you for your help! It pushed me forward with my actual project.

You're my guest for a beer if you pop in Budapest once..

Regards,
TKE
BrolY likes this.
TKE is offline   Reply With Quote

Old   October 7, 2011, 05:21
Default Problem with mesh reading into FLUENT
  #4
TKE
New Member
 
TKE's Avatar
 
Jozsef Rideg
Join Date: Feb 2011
Location: Budapest, Hungary
Posts: 21
Rep Power: 6
TKE is on a distinguished road
Hi,

meantime I have some problem. I recieved an error message in FLUENT with the following words:

"Build Grid: Aborted due to critical error"

"Building...
mesh
Build_Grid: no cells in case file.

I do not know the reason for this problem.
I made a 2D mesh. Converted into unstructured mesh. Extruded with the following options:
New Volume Part Name: FLUID (the same as in 2D)
New Side Part Name: inherited
New Top Part Name: inherited
I have not deleted the original elements. Can it be the source of the problem, or should I search for another reason?

Thank you for your hints!

Regards,
TKE
Attached Images
File Type: png error_FLUENT_mesh_read.PNG (10.7 KB, 21 views)
TKE is offline   Reply With Quote

Old   October 7, 2011, 05:34
Default
  #5
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Thanks for the beer

About your extrude option, be careful with what you have done !
If you let the name of your top and side parts as "inherited", you could have issues when you export your model to fluent. Because your top part would be in the same part than your fluid part. So when you specify your Boundary Conditions (BC), it would put the same BC for your fluid and top part.
The same issue would appear for your side part which would be in the same part than the extruded part.

I don't know if what I'm saying makes sense, so here is an example : I want to mesh a cylinder with an inlet, wall, fluid and outlet parts (all of those parts would have different BC). So first, I mesh the inlet part and extrude it. If I let "inherited part" as top and side part, my inlet part would be in the same part than the wall part. And my outlet part would be in the same part than my fluid. Which is not at all what I want.

Try to change the name of those parts, redo your export and see if it works with fluent. If it doesn't, you should create another thread

Last edited by BrolY; October 7, 2011 at 06:02.
BrolY is offline   Reply With Quote

Reply

Tags
2_dimension, 3_dimension, airfoil, extrusion, icem

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
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 39 June 5, 2013 19:02
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
getting airfoil surface to be recongized for tri mesh josip76 ANSYS Meshing & Geometry 4 June 9, 2011 22:48
[ICEM] Canít get 2D Blayer in hex mesh to be accurate O-block around airfoil josip76 ANSYS Meshing & Geometry 2 June 4, 2011 18:03
2D airfoil optimisation: the mesh Marta Main CFD Forum 5 February 6, 2008 02:07


All times are GMT -4. The time now is 00:48.