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

[ICEM] Problem with mashing NACA0012 2D to 3D

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 29, 2012, 11:26
Default Problem with mashing NACA0012 2D to 3D
  #1
New Member
 
Natalia
Join Date: May 2012
Posts: 7
Rep Power: 5
natala1987 is on a distinguished road
Hi,
I've got big problem with NACA0012 meshing. I do not have experience with CFD and I really need your help I've done 2D mesh and it works in Fluent. Now I should create mesh in 3D with the same parameters (something like extrude for 0.2). I attache my 2D ICEM CFD file.
Thank you for your help
Attached Files
File Type: zip NACA0012.zip (32.7 KB, 43 views)
natala1987 is offline   Reply With Quote

Old   May 29, 2012, 11:30
Default
  #2
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
here is a link of a video tutorial on how to mesh a 3D wing made by Mr Far:
http://www.youtube.com/watch?v=mgjRT4WY_iA
hope it can help
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   May 29, 2012, 11:35
Default
  #3
New Member
 
Natalia
Join Date: May 2012
Posts: 7
Rep Power: 5
natala1987 is on a distinguished road
http://sendfile.pl/171206/NACA0012.zip
http://sendfile.pl/171207/NACA0012_2.zip
natala1987 is offline   Reply With Quote

Old   May 29, 2012, 12:30
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Now I should create mesh in 3D with the same parameters (something like extrude for 0.2)
This option works fine, if you want to simulate the 3d effects for 2d case (quasi 3d with symetry condition on both sides of wing). But if you really want the 3d wing mesh, that is meshing is also going after the wing and also inside the airfoil block exteded in the 3d then you should start with the 3d blocking and or you can make the 2d blocking and revolve it (as pointed by Simon and I am quoting exact words below)

Quote:
There are several ways to handle a 3D wing. This one's key features are a sharp trailing edge (which suggests a C Grid) and a flat wing tip, which is most easily captured with (Blocking => Create => 2D to 3D).

Start with a 2D blocking... But because you will need to keep the flow volume past your wing tip, you also need to mesh inside the airfoil. The topology Far showed works well, or if you can handle wedges in your model, you could just keep the very simple collapsed block you got from collapsing the blocks behind the trailing edge, then add the Ogrid to the front inner block of the airfoil.

Then go to Create Blocks => 2D to 3D and choose the "by translation" option. Put in the width of your box and apply.

Then go and "delete" the blocks that should end up inside the airfoil (or put then in a solid blocking material).

Associate all the edges with the 3D curves, set up edge parameters, etc.

Done.
Detailed procedure is discussced here and diamondx already proivded you the link for YouTube video.
Structured Hexa Mesh on Wing

Blocking is also attached with above post for four different procedures. If you still find it difficult, let us know and we shall help you out.
Far is offline   Reply With Quote

Old   May 29, 2012, 12:32
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I am also going to add the voice in these videos soon.
Far is offline   Reply With Quote

Old   May 29, 2012, 14:06
Default
  #6
New Member
 
Natalia
Join Date: May 2012
Posts: 7
Rep Power: 5
natala1987 is on a distinguished road
Thanks I am going to do it tomorrow and I will let you know ab.results
natala1987 is offline   Reply With Quote

Old   May 31, 2012, 09:50
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
Just to be clear, it is possible to extrude the blocking or the mesh (2.5D), but Far is assuming that you are actually trying to mesh a real 3D wing with a wing tip...

If you really want to mesh the full wall to wall airfoil, extruding what you already have is the easiest way.

Best regards,

Simon
__________________
-----------------------------------------
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   May 31, 2012, 10:29
Default
  #8
New Member
 
Natalia
Join Date: May 2012
Posts: 7
Rep Power: 5
natala1987 is on a distinguished road
My wing is symmetry so "extrude" is easier way than create geometry, blocking...I had problem with "extrude" because my boundary conditions did not work in Fluent, but I solved a problem. Before "extrude mesh" necessary is tick "lines" in mesh tree. Mesh and boundary conditions are working and results of lift and drag coefficient are the same as experimental results
natala1987 is offline   Reply With Quote

Old   May 31, 2012, 10:34
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Actually, if you are trying to include the 3d effects then extrude is the best option. However if you want to solve the 3d wing then you need to consider the 3d blocking.

Can you post the few pics of goemetry, mesh and results.
Far is offline   Reply With Quote

Old   May 31, 2012, 10:46
Default
  #10
New Member
 
Natalia
Join Date: May 2012
Posts: 7
Rep Power: 5
natala1987 is on a distinguished road
No problem but tomorrow, becuse I've back from university
natala1987 is offline   Reply With Quote

Old   June 1, 2012, 04:40
Default
  #11
New Member
 
Natalia
Join Date: May 2012
Posts: 7
Rep Power: 5
natala1987 is on a distinguished road
I can send you few print screens of my mesh. In 3D case I have 4 layer (every one 0.05). It is not too much but it is enough to compare with experimental results. In the next part I will simulate accretion of icing on the airfoil.

I am not sure what mean Area and Length in references value in Fluent? could you help me?
Attached Images
File Type: jpg modyfikacja1qq.jpg (77.3 KB, 26 views)
File Type: jpg modyfikacja1qqqqq.jpg (97.4 KB, 25 views)
File Type: jpg nataliapress3dlaa1.jpg (94.5 KB, 27 views)
File Type: jpg 11.jpg (99.5 KB, 29 views)
natala1987 is offline   Reply With Quote

Old   June 1, 2012, 05:07
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Are you taking 30% of chord to extrude airfoil in 3rd direction? Four nodes may be sufficient I am not sure. Length is air-foil chord and area is the chord * unit because you are simulating the 2d airfoil

Model top and bottom wall with slip condition (zero shear) and dont apply pressure far field.
Far is offline   Reply With Quote

Old   June 1, 2012, 05:19
Default
  #13
New Member
 
Natalia
Join Date: May 2012
Posts: 7
Rep Power: 5
natala1987 is on a distinguished road
I am confused ;/ I should talk with my supervisor. So in your opinion which depth will be the best, 1?

In 3D case to compute area I should multiply chord *depth?
natala1987 is offline   Reply With Quote

Old   June 1, 2012, 05:59
Default
  #14
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
depth should be 0.3*chord to 0.4*chord for the 2d cases with 3d effects. I have learned it from the research paper.

Since you are simulating the 2d cases, therefore you should take the 2d properties to normalise the data.
Far is offline   Reply With Quote

Reply

Tags
icem 3d

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
conduction problem venkataramana OpenFOAM 3 December 1, 2013 08:30
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Problem with airflow over naca0012 and angle o f attack Lucas OpenFOAM Running, Solving & CFD 2 February 18, 2011 14:13
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13


All times are GMT -4. The time now is 01:45.