CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [GAMBIT] multi element wing - mesh problem (

Zweeper March 15, 2010 16:43

multi element wing - mesh problem
hey everybody!

at the moment i'm trying to mesh something for my final year project. i already finished with the 2dimensional analysis of this problem and now i start to analyse a multi element wing in 3 dimensions.

i created the wings with pro engineer, imported them into gambit and created two zones around the wings. the inner zone is used as interior and the outer zone is my "windtunnel".

i wanna mesh it with a t-grid mesh but as soon as i mesh the interior zone, gambit reports problems with highly skeewed elements. I know that i have to avoid them and in a 2d case i know how to do that, but in this 3d case i have really no idea how i can mesh my wings :(

for a better understanding, i attached my gambit files:

hope that someone can help me!

regards, zweeper

-mAx- March 16, 2010 02:04

I can help you, but I have web restriction, so I will be able to check your files only tomorrow.
Once your volume is meshed, do you checked where are the skewed cells? Examine Mesh icon, and set the lower value to 0.9
If you see a bunch of red cells, then you have to find the reason (small edges etc...).
You can post a picture if you don't want to wait,
(if your dbs file is less than 10MB you can mail me it)

Zweeper March 16, 2010 06:25

Hey max, thanks for your answer!
My dbs file is less than 1 mb, if you give me your e-mail address i can send it to you. The problem is that i cant examine my mesh because gambit doesn't creates the mesh. It always occurs an error message before the mesh becomes finally created.

-mAx- March 16, 2010 10:50

okay quick before I leave the office, I saw that the domain containing the flaps, is assigned to be meshed with Hex-Tet Primitive.
Try to mesh it with tet hexcore, but you have to refine your mesh on the trailing edge of the first flap (I guess you know why, you had the same problem with 2d, isn't it?)
There is also a problem with the big volume (connectivity)

Zweeper March 16, 2010 12:35

you mean hex-cooper with hexcore, dont you?

actually i thought the best mesh for me is the t-grid one because it is the only mesh which worked for me so far.

volume error (connectivity)?
hm, i created this geometry with pro-engineer. can i check/fix this connectivity problem with gambit? is there a way?

-mAx- March 16, 2010 12:48

no Tetra with hexcore, it is the quickest way to mesh your volume (it filled your volume with a core of hexa, and the boundaries with tetra) Very powerfull if you don't have time to spend days on a mesh.
You cannot mesh your volume on the fly with hexa.
For your volume issue: delete the upper volume but disable lower geometry.
it will delete the volume but not the surfaces. Then create a volume with those 6 surfaces. Finally split it with the other volume (the one containing the hull).
For checking the connectivity, click on the connectivity icon next to the examine mesh. The interfaces should appear in pink. If not, there is a problem.
Next time, just import the hull from proE, and creates the brick with gambit

Zweeper March 16, 2010 14:30

okay, i did everything you suggested me. at the end all contours (really all of them) are blue. Just the vertexes on the edges are pink, but not the edges itself.

-mAx- March 16, 2010 14:40

then they aren't connected.
Try to split the volume with the 6 surfaces from the smallest volume (enable connectivity).

-mAx- March 17, 2010 02:29

1 Attachment(s)

Originally Posted by -mAx- (Post 250300)
then they aren't connected.

Ok I checked the connectivity and it is ok. Sorry for the mistake
Now regarding your mesh issue. As I said the problem comes from the trailing edges. I don't know what kind of hardware you have, but your mesh will be huge, and you cannot mesh it with only 2 volumes.
For instance I created a cylinder (ellipse based) which surrounds the wings, and I split the small volume with it. Then I meshed it on the fly. The mesh (coarse) is already 1,4 millions big.
There are high skewed cells located at trailing edges, which means that you have to refine your mesh in those areas
Attachment 2615

Zweeper March 17, 2010 06:24

okay all right, i will try it today/tomorrow with your suggested tips.
maybe i can also simplify my geometry at the trailing edges, if not i will try it exactly your way.

So the geometries/volumes are okay? i don't have to modify anything?

I have a dual core 2 GhZ cpu with 3gb ram, you think this could be enough without haning days on this iteration/meshing? ^^

but so far, big big big thanks to you!

-mAx- March 17, 2010 06:55

the connectivity is ok
and you can go and mesh your geometry.
Just pay attention at trailing edges.
I assume your dual Core will suffer... (usually 1 million cells for 1 GB Ram)

Zweeper March 17, 2010 16:03

Thanks, i will try it now.

One general question for a volume (3d) mesh:

did you meshed the edges at first and then the volume? or did you meshed edges, then faces and then the volume?

(the steps to refine the mesh, is it to mesh just the edges or also the faces?)

Zweeper March 17, 2010 18:14

okay, finally it works now.
you where right, my laptop runs on its limit, but i hope the iteration will end... some when... :)

but thanks a lot!!!!

-mAx- March 18, 2010 01:46


Originally Posted by Zweeper (Post 250472)
One general question for a volume (3d) mesh:

did you meshed the edges at first and then the volume? or did you meshed edges, then faces and then the volume?

(the steps to refine the mesh, is it to mesh just the edges or also the faces?)

I mesh the volume directly, but I use Size Functions for refining at vertex, edges or surfaces

Zweeper March 19, 2010 07:58

Okay, i have another question. I meshed it now with t-grid because it worked better/faster for me. But the t-grid option offers me now the following option:

"meshed s.f. on b.l. cap" and i can enter a growth rate and also a max. size.
What exactly does this option do? is it creating a kind of boundary layer around my object?

-mAx- March 19, 2010 09:07

it will be ignored since you don't have any BL.
from the help:"Applying Meshed Size Functions on Boundary Layer Caps When you apply the TGrid meshing scheme to a volume to which boundary layers are attached, you can automatically apply a meshed size function at the boundary layer cap. This capability is invoked by the Meshed S.F. on B.L. cap option on the Mesh Volumes form"

Zweeper March 19, 2010 09:12

okay, thanks for your help.
just asked that because i'm not able to add an boundary layer to my wings. it means that it can just add boundary layers to flat plates, i will try it now without boundary layer and i hope that it is accurate enough as long as my y+ is in the desired range.

-mAx- March 19, 2010 10:28

1 Attachment(s)
Sure you can.

Attachment 2647
I think it creates one, but you cannot see it.
For that, split the volume at each wing extremity. It will enforce the BL to attach the ellipse section, and you will see it.
The problem will be the thickness of your BL especially between the 2 airfoils. If there is BL-intersection, then I would treat this volume separately (with splits) and mesh it with hexa (according to your y+). You can attach BL to other volumel

Zweeper March 29, 2010 09:17

i really dont get this with gambit.
I start having problems with splitting the volume.
i guess you mean i should create a new plane trough the zone where i wanna split the volume, and then split it, is that right?

-mAx- March 30, 2010 00:55

1 Attachment(s)
Create a (xy)-plane, move it with vector (0 0 500).
Split your volume with this plane.
Do the same at the other wing extremity.
Attachment 2736

All times are GMT -4. The time now is 10:32.