blocking 3D wind turbine blade
 

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:o

why i couldn't upload my geometry.tin file?

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 ;)

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?:cool:

this can done. search the cfd online for the detailed steps.

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).

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?

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.

:could you put up suggestions please?:)

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. :)

You should go for Tetra + prism. Atleast for initial run...

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?:confused:

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

are you trying to merge both meshes?

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...

hello far and scipy,

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

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:confused:

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

http://i.imgur.com/ppvX5Ky.jpg?1
http://i.imgur.com/FSPoclz.jpg?1

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