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

[GAMBIT] Structure Mesh for Cyclon

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

Like Tree3Likes
  • 1 Post By masoodina
  • 1 Post By -mAx-
  • 1 Post By Far

Reply
 
LinkBack Thread Tools Display Modes
Old   July 7, 2012, 05:31
Default Structure Mesh for Cyclon
  #1
New Member
 
green iran's Avatar
 
A_A
Join Date: Oct 2010
Posts: 10
Rep Power: 6
green iran is on a distinguished road
Hi
I'm trying to create a structure mesh for the cyclon but with no any progress. I divided the model into several subdivisions. This leads to many internal surfaces which then I defined them as "Interior". When I tried to import the mesh file to Fluent it was showed me a lot of errors with something like this:
Error:Cannot change zone-7 to interior because there is only one adjacent cell thread. Error Object:
Actually, this message was seen for half of the internal surfaces. Afterwards, Those surfaces which had the error turned into wall surface.
I'm really confused and I need some help. I have a few questions:
1-How important it is to create a structure mesh for cyclon?
2-In case we have to use a structure mesh, how can it be generated for a cyclon?
3- should I use multiblock? If so, real or virtual?
Any help will be really appreciated
Attached Images
File Type: png Capture 2.PNG (19.8 KB, 51 views)
green iran is offline   Reply With Quote

Old   July 7, 2012, 07:38
Default
  #2
New Member
 
masood
Join Date: May 2012
Posts: 18
Rep Power: 5
masoodina is on a distinguished road
hi .

once in fluent select the inner faces and change their b.c's to interface .
then define grid interface as coupled . and it will make some shadow walls (in fact no surface) . then chek your grid . it will help .

because of highly swirling flows and les or rsm model u have to have a good structured mesh .
green iran likes this.
masoodina is offline   Reply With Quote

Old   July 9, 2012, 01:55
Default
  #3
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,961
Rep Power: 30
-mAx- will become famous soon enough
Basically you don't need to define internal surfaces as "interior".
If your splits are well done, then volumes are connected, and those surfaces are automatically set as interior (but not visible as bc).
You will have problem, if those surfaces will be automatically set as wall, which means, than volumes aren't connected
You are not enforced to mesh your geometry with hexa. (I can suggest you tetra-hexcore)
Real and/or virtual is only a topology stuff, no influence on mesh
Multiblock is a must for hexa mesh. For tetra, you may do some split for a better mesh control on a mesh, or for example, you want to mesh a volume with hexa, but not the other (typically complexd geometry with inlet-outlet pipe system >> you can isolate both pipes and mesh them with hexa)
green iran likes this.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 9, 2012, 02:37
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,905
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
leads to many internal surfaces which then I defined them as "Interior"
There is no need to define them internal, by default they are internal if you not specify the boundary condition and they have fluid on both sides.


The video tutorial given below presents the meshing of cyclone in ICEM CFD. But still you can get an idea about the blocking that how to split your geometry in gambit to get the similar mesh.

What I can suggest you is to extend the upper geometry topology where you have created very nice splits for the o-block meshing inside the pipe down to the bottom. Also edges outside and inside the pipe should be connected at the same vertices.

For tangential inlet, you can divide into into two volumes. For triangular you can use Tri Primitive http://202.118.250.111:8080/fluent/G...ide/mg0303.htm(equivalent to Quarter O-grid/Yblock in ICEM) and for rectangular part you can simply use mapped hexa.

use these keywords in Google to find the tutorial on cyclone meshing in ICEM CFD
Quote:
structured mesh generation using ICEM CFD
green iran likes this.
Far is offline   Reply With Quote

Old   July 11, 2012, 11:04
Default Cyclon structure mesh
  #5
New Member
 
green iran's Avatar
 
A_A
Join Date: Oct 2010
Posts: 10
Rep Power: 6
green iran is on a distinguished road
Hello again guys
Eventually, I solved my problem. The problem was regarding to the way of splitting, Something I never thought of it. Actually, I had forgotten to check connect box option. It was a good experience but took about one week.
Anyway, I really appreciate you for your precious and constructive comments.
__________________
Regards Yours
green iran 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
Number of cells in mesh don't match with size of cellLevel colinB OpenFOAM Native Meshers: snappyHexMesh and Others 11 January 13, 2015 12:47
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
mesh data structure for zone connectivity Xiaoming Main CFD Forum 0 March 7, 2005 16:33


All times are GMT -4. The time now is 07:21.