Meshing sinusoidal leading edge wing in ICEM
 

Hi there,

I am trying to mesh a wing which has sinusoidal leading edge and so far have been struggling with the mesh. I would like to know if I should use an O-grid block or a C-grid. I tried to use a C-grid and the resulting mesh has a lot of errors. I am attaching my project files. I want to use symmetry boundary conditions on both sides of my model (wing modeled as an infinite wing) . Please help me out thanks.

Hey this is what I got on your case in 10 minutes. Hope it helps you...

http://www.cfd-online.com/Forums/att...curveswing.jpg

https://dl.dropbox.com/u/68746918/Tubercle_all_far.rar

https://dl.dropbox.com/u/68746918/Tubercle_Far.zip

PS: Upload on dropbox may take some time, meanwhile you may encounter error 404

Hi Far,

Thank you very much for helping me out. I will learn from your blocking strategy and if I come across any trouble i'll post again. Thanks again I really appreciate your help.

You will notice that I have divided surface of wing into four parts (arbitrarily at 25%, 50% and 75% spanwise locations). I don't know why ICEM likes this way of surface in blocking and recently I happen to solve similar in following thread with this method of surface division.

http://www.cfd-online.com/Forums/ans...m-meshing.html

PS: This may not be the actual issue, it may be just my illusion.:confused:

Hi there,

May I know how were you able to extract curves from surfaces? It seems like you generated the airfoil sections in the middle and one on each sides. I tried to use extract surfaces from curves options in geometry and have been unsuccessful.

Geometry > Create/Modify curve > Iso curve methods (fourth from left in first row)

To split surface : Geometry > Create / Modify Surface > Segment Surface (third from left in 2nd row)

Hi,

were you able to get the trailing edge points perfectly or you manually drew them? because i am unable to project trailing edge curve from above options

Ok. For one surface on trailing edge , I changed parameter from u to v (used same values i.e. 0.25, 0.5 and 0.75). Then I go back to geometry > create point > curve ends (first from left in 2nd row)

Thanks for your help. Using your method I was able to generate a nice grid for my geometry. The thing is I shall be adding more tubercles (image attached). From your experience would you recommend using the same blocking strategy?

I also read the posts you referred earlier regarding 'mesh unable to follow curved geometry'. Unfortunately the project files are not there any more and I have nothing to refer. Please advise.

Same strategy would work perfectly. Re-use same blocking and increase no of nodes on the high curvature areas to capture them properly. Try and come back if you get any problem.

And good luck with your optimization work.

I have those files, but it would be better to ask the primary source Ananthakrishnan.A.S (through pm) to give you files and his thesis. He got the wonderful results for his optimization work.

Look for files in this thread http://www.cfd-online.com/Forums/ans...take-mesh.html

Hi, I'm working on a similar project myself and have been using the ansys mesher mesh it for me. I have been fighting it the whole time trying to generate a nice mesh so I started investigating ICEM.

I have gotton as far as being able to mesh a 3d wing with some sort of success (I think)....but still not quite good enough. How hard would it be to learn how to block like you have for this wing. Ultimately my aim would be to be able to use a script to import the geometry and the (judging by the blocking you have done) input how many nodes so you can use geometry with various amplitudes and wavelengths.

Would it be possible to outline how you blocked this in simple enough terms for an idiot to understand? I understand what youve done in terms of blocking approach, Im just not sure how to achieve it exactly.

Usually I would take more time to learn it thoroughly...but its very late into the project. I would probably spare 2-3 full days learning if I need too, but I cant spend much more then that as I need to keep simulating.

So any chance of a bit of a walk through, or will it not be worth it?

Hi there,

I followed your method and was able to obtain the grid for the case where the amplitude was reduced, however, for the case where amplitude was increased, mesh started to have negative elements. The same goes for the case where the I increased the wavelength. I see some elements penetrating into surface and moved some vertices but didnt help. Would you please mind helping again?

The files are in the link below:

https://www.dropbox.com/s/xcbsri1gin...e_0.5cwave.rar
https://www.dropbox.com/s/t6a383tkfh...rcle_0.15c.rar

did you change "project face" to "project edge"? Right click in premesh to change that and see if that helps.

I tried but it has to do with mesh quality, which is irrespective of projecting edges or faces, which is less than zero in my case.

Stuart: do you still need help? I missed this one as I was busy with my course (renewable energy)

ryerson_guy: please post some pics....

Hey man,

Just had a look and saw how you were doing it. I actually do mine differently (on the advice of FAR) I dont bother splitting the blocks in the spanwise direction. I just associate the leading edges to a curve on the wing to the a single block.

I dont think it captures the geometry perfectly, it seems pretty robust.

Im not sure if I explained that particularly well but here is one of mine for you too look at. You may need to "project to edge" like I said before to see what it will normally look like (for some reason default is set to project to face)

https://www.dropbox.com/sh/b7wxg12rylbw169/s44uwEe1Fh

Hahaha, thanks FAR but you already helped me HEAPS in this thread. (which might be useful to you too ryerson_guy

http://www.cfd-online.com/Forums/ans...edge-wing.html

Hi,

Pics are attached.

Last pic is attached

Showpony I have tried that method before but didn't work out for me.

What problems did you have with it last time? I might have had the same issues. I spent ages getting it to work properly (though it was my first time using ICEM lol)
I started of doing it the same way you did but found it too tedious and not worth it as I could get the same (or better) results doing it without splitting the block in the spanwise direction.

I will have another look in a moment, but I have a feeling that FAR will be much more help to you than I will be. But I will Try :)

One thing I have notices is that you do not have many elements in the spanwise direction. You are barely going to capture the geometry with 8 elements across let alone get any decent resolution of your flow. It will up your element count A LOT but really is probably necessary. If you want to reduce node count you might have to consider a hybrid mesh.

I know in my simulations there is definite 3D flow effects, so if you want to capture them you are definitely going to have to increase the element count in the spanwise direction.

I increased the node count to 12 across each block in the spanwise direction and then projected to edges as mention earlier and I had no problems with volume errors.

https://www.dropbox.com/s/00ft3ejsjz...%20%282%29.zip


Also, if you separate the walls you called symmetry into symmetry1 and symmetry2, you can turn of one of the walls and get a much clearer idea of what is happening with the mesh (because you dont get all that extra interference).

Make sure you renumber the nodes and reduce the bandwidth too if you are struggling to deal with teh extra amount of nodes. Should help a bit.

Sorry the files that I uploaded and the one the pics have a mismatch. The pic has 40 elements along the span, where as the files have less. I still get the same error whenever I try to improve.

Does the way your geometry was drawn and imported to ICEM matters? The initial one and the ones i uploaded were drawn and imported a different way.

Not sure what you are talking about man. Did you even look at either of the files I sent you? 40 elements across is not enough. I ended up doing 12 element on each of the blocks. ie. 12x8=96nodes on the spanwise direction.

I got that rar file you uploaded working fine by doing what I said. the "tubercle_0.5cwave"

The "tubercle_0.2cwave" hasnt been blocked or anything so Im not sure what was going on there.

All I did was increase the amount of spanwise nodes significantly and change the premesh from "project to face" to "project to edge". Literally all I did. Ran the check and there were no errors.

So you just increased the elements in my files as well as projecting edges thats it?

You didnt change my blocking method?

Didnt change blocking, just increased the elements in my files as well as projecting edges and it seemed to work nicely for me.

Would you mind uploading the file please? I am doing the same thing as you and yet having errors again

That said, I still wouldnt bother splitting your blocks like that. It is pretty much a waste of time. can get the same results without splitting it in the spanwise direction

I already did it earlier

but here it is again

https://www.dropbox.com/s/00ft3ejsjz...%20%282%29.zip

EDIT: You mean the same thing with the increasing spanwise nodes and projecting to edge?

Yes increasing spanwise nodes and projecting edges. The link to the file doesnt work.

See if that works now

https://www.dropbox.com/s/00ft3ejsjz...%20%282%29.zip

problem in geometry

Thanks for the upload, but i still see some negative determinants elements although they are very small. Are you using Fluent to run your cases?

Far is there a way I can look for geometry errors in ICEM?

I was running the check in ICEM. I found that if I have no problems in icem then I will have no problems in CFX.

Why it is not projecting to geometry?