CFD Online URL
[Sponsors]
Home > Forums > FLUENT

wind machine mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 11, 2010, 14:19
Default wind machine mesh
  #1
New Member
 
miguel
Join Date: Jan 2010
Posts: 11
Rep Power: 6
miguel.soto is on a distinguished road
Hello everybody

I´m getting lot of trouble to mesh a three-bladed wind machine, without nacelle, using gambit

I started to mesh each blade, giving 100 nodes at radial direction and 30 nodes at tip and hub profiles. Then i mesh each blade face using "quad" elements, "map" type. The far field boundary is made of a cylindrical surface. When i try to mesh the 3d volume a message appears to me, saying " initialization failed, pertutrb boundary nodes and try again...check the skewnesses of your face meshes...". I guess the mistake could be based upon as r/R value increases, distance between nodes decreases.

I also try to mesh blades, using "quad/tri" elements, "pave" type, and equal distance between nodes at tip and hub profiles, but the outcome surface was a non-smoothed surface, so it´s not valid for me.

Actually, i don´t know what more can i do, can you please help me giving some tips/ advices, to solve this problem.

Thanks in advance
miguel.soto is offline   Reply With Quote

Old   January 12, 2010, 01:49
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
Are you trying to mesh your domain with hexa or tetra?
Usually that kind of message comes from a small edge, small angle etc...
Once you have meshed your surfaces, check the 2d-mesh quality and see worst elements (Those cells may give you some trouble)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   January 12, 2010, 12:48
Default
  #3
New Member
 
miguel
Join Date: Jan 2010
Posts: 11
Rep Power: 6
miguel.soto is on a distinguished road
Thanks for your help Max. I have already done some meshes made of tetra, hybrid, hexa. But i guess that the mistake is on meshed faces at blades. What can i do to mesh blade faces on a pave distribution, and get a smooth meshed surface all along the blade? Because i think it´s not possible to mesh that kind of surfaces using a map distribution, it would be good to keep distance between nodes at tip and hub.

Thanks a lot
miguel.soto is offline   Reply With Quote

Old   January 13, 2010, 01:37
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
Post a picture
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   January 13, 2010, 01:56
Default
  #5
Senior Member
 
herntan's Avatar
 
YH Tan
Join Date: Mar 2009
Location: Malaysia
Posts: 118
Rep Power: 7
herntan is on a distinguished road
Picture please.
If u have the surface meshed and fail to mesh to volume, i think u should give up the surface mesh.
__________________
Herntan,

Add Reputation if I am right
herntan is offline   Reply With Quote

Old   January 13, 2010, 13:51
Default
  #6
New Member
 
miguel
Join Date: Jan 2010
Posts: 11
Rep Power: 6
miguel.soto is on a distinguished road
[IMG]file:///C:/Documents%20and%20Settings/miguel%20angel%20soto/Escritorio/Dibujo.JPG[/IMG]
Attached Images
File Type: jpg Dibujo.JPG (35.4 KB, 27 views)
File Type: jpg hub.jpg (104.1 KB, 27 views)
File Type: jpg tip.jpg (104.2 KB, 24 views)
File Type: jpg pave.jpg (102.9 KB, 25 views)

Last edited by miguel.soto; January 13, 2010 at 14:31.
miguel.soto is offline   Reply With Quote

Old   January 14, 2010, 01:58
Default
  #7
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
In your case you only have one volume. And you won't be able to mesh it with hexa on the fly.
That means, that your surface mesh with pave or hexa won't bring you anything.
I would advise you to mesh your blades surfaces with tetra, AND a element size at least 10 times smaller that the actual one. (you aren't able to mesh your volume because of a too coarse surface mesh).
Then apply a size function (type meshed) and choose your blade surfaces as source.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   January 14, 2010, 02:25
Default
  #8
Senior Member
 
herntan's Avatar
 
YH Tan
Join Date: Mar 2009
Location: Malaysia
Posts: 118
Rep Power: 7
herntan is on a distinguished road
Max was right. its the surface meshing limited ur volume meshing.
If u don't need different volume mesh size in your volume, you should give up meshing the surface. I guess if u directly goes for volume mesh, ur meshing should be done easily.
__________________
Herntan,

Add Reputation if I am right
herntan is offline   Reply With Quote

Old   January 14, 2010, 19:13
Default
  #9
New Member
 
miguel
Join Date: Jan 2010
Posts: 11
Rep Power: 6
miguel.soto is on a distinguished road
I have just finished trying to mesh the volume by using smaller element sizes, about three times smaller than the previous one, but still the same message appears, and it doesn´t looks like to be the right direction. If i do it, meshing with ten times smaller elements i will have some trouble to solve the case in fluent, due to iteration time.

The airfoil profile is made up of three curves, upper surface, lower surface, both join by a third line, in the same way as a gourney flap,
Attached Images
File Type: jpg Dibujo.JPG (19.9 KB, 14 views)
miguel.soto is offline   Reply With Quote

Old   January 15, 2010, 02:13
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,861
Rep Power: 29
-mAx- will become famous soon enough
your mesh is still too coarse.
Your trailing edge enforces you to refine your mesh.
It should be the smaller edge from your model, and it is quite important (you cannot merge it).
Thus, I assume you want to resolve the wake from the airfoil.
Check the length from the trailing edge and give it as reference element size of your surface mesh. But it will be still too coarse, because it means you will resolve the wake with one element.
Anyway it should solve your mesh problem.
Then iterate, and try to refine with 8 element along the trailing edge.
Solving CFD will always ask time to iterate (don't expect to get your result in 5min, excepts if you have a CRAY or someting like that).
Your model seems to be periodic, you can compute only a slice and therefore refine your mesh
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   January 20, 2010, 10:58
Default
  #11
New Member
 
Join Date: Dec 2009
Location: Germany
Posts: 6
Rep Power: 7
wake2e is on a distinguished road
Hi,
looks like an Enercon turbine. We made some windturbine meshes with Gambit.

I think that will never work at that way. You have to cut your big Volume in much more smaller volumes and you should try to mesh only one 120 degree part and copy it.
wake2e is offline   Reply With Quote

Old   January 21, 2010, 12:41
Default
  #12
New Member
 
miguel
Join Date: Jan 2010
Posts: 11
Rep Power: 6
miguel.soto is on a distinguished road
thanks for your advice, i will try to do it meshing only 120 degrees. In this way the iteration time shall be at least less than computing the full volume.
miguel.soto is offline   Reply With Quote

Old   January 21, 2010, 12:55
Default
  #13
New Member
 
Join Date: Dec 2009
Location: Germany
Posts: 6
Rep Power: 7
wake2e is on a distinguished road
hi,
no, for resonable results you have to do the full 360 degree, but you can copy and connect the mesh in gambit.

And you should try to use hexaeder, because with tetraeder you will get really a lots of elements.

Here is an older paper, there we used tetraeder meshing in gambit and then convert to polygon-cells in Fluent:
http://www.iop.org/EJ/abstract/1742-6596/75/1/012033/

But I think hexaeder are the best way.

What kind of job are you doing there with the windturbine?
wake2e 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
wind turbine rotor 3D mesh tutorials sivarama1 CFX 2 September 9, 2013 10:23
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 05:24
vtk mesh or Abaqus mesh to OpenFOAM bigphil Open Source Meshers: Gmsh, Netgen, CGNS, ... 19 August 16, 2011 05:14
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 19:10
Mesh Mignard FLUENT 2 March 22, 2000 06:12


All times are GMT -4. The time now is 05:30.