CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

walls that should be interior

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2012, 21:10
Default walls that should be interior
  #1
Member
 
nazareno mancinelli
Join Date: Mar 2009
Location: argentina
Posts: 35
Rep Power: 8
yochule is on a distinguished road
hi guys. i'm working in a VAWT. i did make the mesh in gambit and imported it into fluent. the problem is that i have some interior faces and when i imported the mesh i have walls instead of interior bc.

i have two main zones: the one that its' close to the blades and the other one that's away. i set up a interface in between this two because the interior one is moving while the exterior is fixed. (first attachment)

the problem is in the interior zone. i split the interior face into a lot of faces, so i can have control on the mesh close the airfoil. i liked every straight edges in around the blades so i have "interior bc" when i import the mesh into fluent.
but, with the circular edges i can not link it (because they are not coincident). so as result i have a wal (like this in red thick line in the second attachment).

one solution is to set it as interface without setting the periodic or coupled options. as result i have a lot of errors concerning to this interfase (third screenshot)

what shoul i do? can anybody help me?
thanks!
Attached Images
File Type: jpg Pantallazo.jpg (94.3 KB, 41 views)
File Type: jpg Pantallazo-1.jpg (100.1 KB, 40 views)
File Type: png Pantallazo-2.png (17.4 KB, 32 views)
yochule is offline   Reply With Quote

Old   January 20, 2012, 02:03
Default
  #2
Senior Member
 
Join Date: Mar 2009
Location: Indiana, US
Posts: 185
Rep Power: 8
delaneyluke is on a distinguished road
One problem could be that you have 2 overlapping surfaces at that region and hence FLUENT considers both as walls, try and locate these 2 surfaces and fuse them, FLUENT will automatically create the fused surface as an interior.

Regards
Luke
delaneyluke is offline   Reply With Quote

Old   January 20, 2012, 18:55
Default the solution! and extra question
  #3
Member
 
nazareno mancinelli
Join Date: Mar 2009
Location: argentina
Posts: 35
Rep Power: 8
yochule is on a distinguished road
i could not do that, in the zone list to fuse, i just have the options for inlet, oulet, blades, interfase1, interfase2 and the wall (the inner edges close the blades). so, because i don't have the interior fluid zone in this list i can not fuse it with this walls.
i did do the next. i go back some steps in gambit, and split every circle of the fluid zone in such of parts as i have in the "close to the blades" zones. so i have a circle maded with some (5) arcs pieces. them, i linked every arc with the face's arc around the blade fluid zone. the result work fine when i imported it in fluent.

by the way, i did run the problem in fluent and i have like a error zone close to the interface (i think). i did make a mesh refinement and the weird velocity distribution persist. what should i do?
Attached Images
File Type: jpg Pantallazo.jpg (17.9 KB, 15 views)
File Type: jpg Pantallazo-1.jpg (37.6 KB, 18 views)
yochule is offline   Reply With Quote

Old   January 23, 2012, 03:06
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
connection problem.
To persuade you: in gambit select one small disk and move it with a translation vector.
If gambit does it without error, then your 2 domains aren t connected (and then at the "interface" between both domains, you have superposed edges (circles) treated as wall in Fluent.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   January 23, 2012, 14:11
Default
  #5
Senior Member
 
Join Date: Jun 2011
Posts: 108
Rep Power: 6
mali28 is on a distinguished road
Quote:
Originally Posted by yochule View Post
i could not do that, in the zone list to fuse, i just have the options for inlet, oulet, blades, interfase1, interfase2 and the wall (the inner edges close the blades). so, because i don't have the interior fluid zone in this list i can not fuse it with this walls.
i did do the next. i go back some steps in gambit, and split every circle of the fluid zone in such of parts as i have in the "close to the blades" zones. so i have a circle maded with some (5) arcs pieces. them, i linked every arc with the face's arc around the blade fluid zone. the result work fine when i imported it in fluent.

by the way, i did run the problem in fluent and i have like a error zone close to the interface (i think). i did make a mesh refinement and the weird velocity distribution persist. what should i do?

You have to connect the faces that are overlapping, otherwise when you export the mesh Fluent will treat the overlapping faces as wall.
mali28 is offline   Reply With Quote

Old   January 23, 2012, 17:33
Default
  #6
Member
 
nazareno mancinelli
Join Date: Mar 2009
Location: argentina
Posts: 35
Rep Power: 8
yochule is on a distinguished road
hi guys
-mAx- : that's a good way to be sure about that. i did fix the problem (last post), but i'd try your suggestion and it's totally true: you can not move it if it is connected.
mali28: thanks. but i'd know which the problem was. the issue it was that i did not make any idea how to fix it. but i finally did.

so, muchas gracias chi@os. suerte con sus simulaciones!
yochule is offline   Reply With Quote

Reply

Tags
boundary conditions, interface, interior, vawt, wall

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
[ICEM] Shadow walls in Fluent. ICEM meshes vs Workbench aarvay ANSYS Meshing & Geometry 10 February 5, 2014 12:17
Importing a mesh from Gambit Interior faces that are walls gschaider OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 84 September 11, 2011 03:27
Problem with rhoSimpleFoam : exploding enthalpy and density at the walls david39 OpenFOAM Running, Solving & CFD 6 January 18, 2011 12:49
Boundary conditon about interior zhou FLUENT 0 September 19, 2003 18:00
thermal conditions of walls Stefan FLUENT 2 March 23, 2003 07:17


All times are GMT -4. The time now is 19:44.