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

[ICEM] blocking 3D wind turbine blade

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

Like Tree7Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 11, 2016, 00:23
Default blocking 3D wind turbine blade
  #1
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
hello everyone,

i have problem in meshing my wind turbine blade, i have followed the conventional C-grid blocking as shown in https://www.youtube.com/watch?v=EknKVAJGEJ8 but it works best with straight blade. PLEASE have a look at my geometry and advice on how to solve it
Attached Images
File Type: jpg 3d_blade.jpg (19.7 KB, 46 views)
chuky_abc is offline   Reply With Quote

Old   March 11, 2016, 00:29
Default
  #2
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
why i couldn't upload my geometry.tin file?
chuky_abc is offline   Reply With Quote

Old   March 12, 2016, 18:48
Default
  #3
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 188
Rep Power: 8
scipy is on a distinguished road
Send a message via Skype™ to scipy
ICEM CFD 3D wing blocking

However, if your blade has a sharp trailing edge and a rounded tip (dome of some sort) you can forget about blocking out a hexa mesh. Either simplify to a truncated (straight cut-with-a-plane) tip or switch to some unstructured meshing approach.

Good luck
chuky_abc likes this.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   March 13, 2016, 00:49
Default
  #4
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
hi scipy, thanks for your reply.

Is tetra mesh considered unstructerd? because i just did it for my blade as in the picture. is it possible to make hybrid mesh where the far field hexa and the blade tetra?
Attached Images
File Type: jpg tetra.jpg (77.6 KB, 43 views)
chuky_abc is offline   Reply With Quote

Old   March 13, 2016, 01:14
Default
  #5
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
this can done. search the cfd online for the detailed steps.
chuky_abc likes this.
Far is offline   Reply With Quote

Old   March 13, 2016, 04:47
Default
  #6
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 188
Rep Power: 8
scipy is on a distinguished road
Send a message via Skype™ to scipy
As Far said, this is doable. You can take several approaches to achieve it:

1. a fully conformal hexacore mesh (which is doable in FLUENT Meshing, look into the FLUENT Meshing tutorial guide - there's a tutorial on hybrid viscous meshing for a car shape followed by a hexacore approach tutorial for the same geometry),
2. you can go for a fully conformal merged mesh in ICEM CFD (creating two volumes of fluid, meshing the region near the blade with tetra and inflating prisms, then meshing the rest of the domain by blocking out a fully structured hex mesh and finally merging the two meshes at the interfaces - there's a tutorial in the ICEM CFD tutorial guide on a hybrid tube mesh that deals with this).
3. you could basically repeat the 2nd option but without any merging and just specify a non-conformal interface in FLUENT.

However, from looking at your screenshot the first thing you should do is increase the size of the domain because you'll never achieve any results in the solver with a domain this small. Make it at least 3-5 blade lengths in each direction (even more is usually done, but for start 3-5 should be enough).
chuky_abc likes this.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   March 13, 2016, 05:39
Default
  #7
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
woaa thanks scipy for your effort,

Actually my domain looks like below where it is 120 degree with the blade in the middle which i just tried to (tetra with hexa core mesh) by following the tutorial from ICEM cfd.

for your suggestion is it applicable for this kind of domain? i mean isn't structured mesh require the blocking and the tetra doesn't

if i continue with full unstructured mesh will it bear the same result?
Attached Images
File Type: jpg domain.jpg (176.5 KB, 24 views)

Last edited by chuky_abc; March 19, 2016 at 18:34. Reason: image hosting problem
chuky_abc is offline   Reply With Quote

Old   March 13, 2016, 05:51
Default
  #8
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 188
Rep Power: 8
scipy is on a distinguished road
Send a message via Skype™ to scipy
Your domain looks OK (maybe the inlet face could be a bit more distanced from the blade) and that blue region just serves as a "refinement box" for the area around the blade (I'm guessing). This is all OK.

Yes, structured mesh requires blocking. The idea here would be that you mesh the rest of your domain (everything except the blue volume) with hexahedrals and then merge these two meshes at the interfacing zones. This would save up on element count and provide superior wake resolution etc.

However, this is a bit complex and unstructured mesh will provide you with decent results if you refine it where it's necessary (around the blade and in the wake of the blade). You could even do these refinements later on in the solver through mesh adaptations based on pressure/velocity gradients.

Basically, if you've got enough RAM available to run unstructured tetra meshes of decent element counts, then do this.. it's much simpler and less time consuming.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   March 13, 2016, 07:50
Default
  #9
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
:could you put up suggestions please?
chuky_abc is offline   Reply With Quote

Old   March 13, 2016, 08:28
Default
  #10
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 188
Rep Power: 8
scipy is on a distinguished road
Send a message via Skype™ to scipy
I gave you a whole bunch of suggestions... If you want others to do work instead of you, that's over at the CFD Freelancers part of the forum.
chuky_abc likes this.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   March 13, 2016, 11:05
Default
  #11
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
You should go for Tetra + prism. Atleast for initial run...
chuky_abc likes this.
Far is offline   Reply With Quote

Old   March 13, 2016, 12:16
Default
  #12
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
thanks scipy and far,

i did what you suggested and here (hexa + tetra), at first it looks OK then it looks distorted when i smoothed it because the quality need to be higher than 0.3 in FLUENT right?

also when i set up the boundary condition to periodic (which marked with pink) it failed to load to fluent




Quote:
Originally Posted by scipy View Post

Yes, structured mesh requires blocking. The idea here would be that you mesh the rest of your domain (everything except the blue volume) with hexahedrals and then merge these two meshes at the interfacing zones. This would save up on element count and provide superior wake resolution etc.
Attached Images
File Type: jpg hybrid.jpg (177.1 KB, 16 views)

Last edited by chuky_abc; March 19, 2016 at 18:28. Reason: image hosting problem
chuky_abc is offline   Reply With Quote

Old   March 13, 2016, 14:49
Default
  #13
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
are you trying to merge both meshes?
Far is offline   Reply With Quote

Old   March 13, 2016, 18:33
Default
  #14
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
yes, i made the tetra first > save mesh > close mesh > blocking > save blocking
> open tetra meah > pop up ask to merge and i pressed merge button > edit mesh> merge surface

Quote:
Originally Posted by Far View Post
are you trying to merge both meshes?
chuky_abc is offline   Reply With Quote

Old   March 13, 2016, 22:21
Default
  #15
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by chuky_abc View Post
yes, i made the tetra first > save mesh > close mesh > blocking > save blocking
> open tetra meah > pop up ask to merge and i pressed merge button > edit mesh> merge surface

No Dont do that. As scipy said in earlier post do not fuse them...
chuky_abc likes this.
Far is offline   Reply With Quote

Old   March 17, 2016, 02:25
Default
  #16
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
hello far and scipy,

thanks for your efforts, btw my lecturer want me to make the mesh to be structured, attached is my geometry file. the pre-mesh have low quality please advice me how to fix it. i have been searching other threads with the same case as mine too.https://www.dropbox.com/s/qcs2r3fnnn...egree.zip?dl=0
Attached Images
File Type: jpg snap.jpg (30.8 KB, 15 views)

Last edited by chuky_abc; March 19, 2016 at 18:36.
chuky_abc is offline   Reply With Quote

Old   March 17, 2016, 04:47
Default
  #17
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,314
Blog Entries: 6
Rep Power: 43
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by chuky_abc View Post
hello far and scipy,

thanks for your efforts, btw my lecturer want me to make the mesh to be structured, attached is my geometry file. the pre-mesh have low quality please advice me how to fix it. i have been searching other threads with the same case as mine too.https://www.dropbox.com/s/qcs2r3fnnn...egree.zip?dl=0


Appraoch for this case is almost similar to wing meshing. check videos on youtube. I have also placed one there. hope it will be helpful. Meanwhile i will also check your file.
chuky_abc likes this.
Far is offline   Reply With Quote

Old   March 17, 2016, 07:15
Default
  #18
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
Quote:
Originally Posted by Far View Post
Appraoch for this case is almost similar to wing meshing. check videos on youtube. I have also placed one there. hope it will be helpful. Meanwhile i will also check your file.
i will check it asap, the i will update my mesh
chuky_abc is offline   Reply With Quote

Old   March 18, 2016, 11:47
Default
  #19
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
Quote:
Originally Posted by Far View Post
Appraoch for this case is almost similar to wing meshing. check videos on youtube. I have also placed one there. hope it will be helpful. Meanwhile i will also check your file.
hi far,

i have tried your blocking strategy on flat plate version of my blade as practice. the low quality elements seems to be on the hub area,the trail, and floating

do i need to adjust the edge parameter or is it because of my domain. i will try it on my real blade and update later. thanks for the video


chuky_abc is offline   Reply With Quote

Old   March 19, 2016, 11:42
Default
  #20
New Member
 
shuk
Join Date: Feb 2016
Location: malaysia
Posts: 28
Rep Power: 2
chuky_abc is on a distinguished road
hello far,

after checking out your videos i have tried my best to block my blade, unfortunately the quality is not satisfying. i have followed your steps carefully.

the second o-grid edges doesn't seems to fit into the my airfoil shaped wind turbine, kindly please have a look at my latest mesh and tell me what i did wrong

thanks

https://www.dropbox.com/s/u3wpwzeprj86dcg/try.zip?dl=0
chuky_abc 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
please help in simulating a wind turbine blade in 6 DOF ????.... usman naseer Main CFD Forum 2 March 10, 2016 03:53
Anlysing and Calculating the power output from a wind turbine blade mrswordf1sh FLUENT 0 March 9, 2015 10:27
Problem in conducting CFD of analysis of wind turbine blade atulpat CFX 16 August 17, 2013 04:09
Wind Turbine Blade rotation mmd_knr FLUENT 1 August 8, 2012 14:52
Wind Turbine Blade Geometry SeanieB Main CFD Forum 0 November 27, 2009 11:18


All times are GMT -4. The time now is 14:19.