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

[GAMBIT] multi element wing - mesh problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 15, 2010, 16:43
Default multi element wing - mesh problem
  #1
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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:
http://rapidshare.com/files/363795841/3D.rar


hope that someone can help me!


regards, zweeper
Zweeper is offline   Reply With Quote

Old   March 16, 2010, 02:04
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
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)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 16, 2010, 06:25
Default
  #3
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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.
Zweeper is offline   Reply With Quote

Old   March 16, 2010, 10:50
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
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)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 16, 2010, 12:35
Default
  #5
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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?
Zweeper is offline   Reply With Quote

Old   March 16, 2010, 12:48
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 16, 2010, 14:30
Default
  #7
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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.
Zweeper is offline   Reply With Quote

Old   March 16, 2010, 14:40
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
then they aren't connected.
Try to split the volume with the 6 surfaces from the smallest volume (enable connectivity).
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 17, 2010, 02:29
Default
  #9
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
Quote:
Originally Posted by -mAx- View Post
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
Sans titre.jpg
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 17, 2010, 06:24
Default
  #10
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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!
Zweeper is offline   Reply With Quote

Old   March 17, 2010, 06:55
Default
  #11
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
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)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 17, 2010, 16:03
Default
  #12
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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 is offline   Reply With Quote

Old   March 17, 2010, 18:14
Default
  #13
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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!!!!
Zweeper is offline   Reply With Quote

Old   March 18, 2010, 01:46
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
Quote:
Originally Posted by Zweeper View Post
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 19, 2010, 07:58
Default
  #15
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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?
Zweeper is offline   Reply With Quote

Old   March 19, 2010, 09:07
Default
  #16
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
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"
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 19, 2010, 09:12
Default
  #17
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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.
Zweeper is offline   Reply With Quote

Old   March 19, 2010, 10:28
Default
  #18
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
Sure you can.

Sans titre.jpg
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
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   March 29, 2010, 09:17
Default
  #19
Member
 
smith
Join Date: Apr 2009
Posts: 75
Rep Power: 7
Zweeper is on a distinguished road
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?
Zweeper is offline   Reply With Quote

Old   March 30, 2010, 00:55
Default
  #20
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,789
Rep Power: 28
-mAx- will become famous soon enough
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.
Sans titre.png
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- 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
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55
Gambit problems Althea FLUENT 21 February 6, 2001 07:05
Mesh Mignard FLUENT 2 March 22, 2000 05:12
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 10:09


All times are GMT -4. The time now is 14:21.