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

[GAMBIT] 3D Two pipe T-shape junction mesh

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

Like Tree1Likes
  • 1 Post By -mAx-

Reply
 
LinkBack Thread Tools Display Modes
Old   April 25, 2013, 07:53
Question 3D Two pipe T-shape junction mesh
  #1
New Member
 
Jing Shi
Join Date: Feb 2013
Posts: 20
Rep Power: 4
Jing is on a distinguished road
Hi everyone,

I am drawing a 3d 2 pipe T-shape junction mesh. I mainly followed the method described in Gambit manual about the 3 pipe intersection. Now, I have finished to interface mesh building, as shown in the figure attached. My problem is when I meshed the volume(i.e. the three pipes), using cooper and Hex/Wedge for the scheme, no matter which interval count I specified in spacing, the meshed volume is always the same with the default spacing (i.e. interval size 1) which is too denser for me. I tried to draw an edge on the pipe surface and meshed that edge first, hoping the volume meshing could follow that spacing on the edge, but it did not work.

Could anybody give me some instruction I can I get a volume mesh with a specified spacing along the pipe direction? Many Thanks!

Regards,
Jing
Attached Images
File Type: jpg 2 pipe intersection.jpg (32.4 KB, 65 views)

Last edited by diamondx; April 26, 2013 at 14:59.
Jing is offline   Reply With Quote

Old   April 25, 2013, 09:15
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
If your splits are well done, you should have 3 volumes, for your 3 pipes.
Now as you already did, you need to mesh the "interface" surfaces first.
Then just pick a volume, and mesh it with Cooper (it should be automatically selected, if not you may enforce it, and you need to specify your sources: 3 surfaces in your case (2 from (interfaces" and the opposite cap)).
Once it is done (meshed), check how looks like the opposite cap's mesh. It should have same size then your meshed sources (since it is a cooper projection).
If not, then something is wrong, and I would gamble on face connectivity at t-junction.
The element size parameter in the volume mesh influences only the mesh in the axial direction; which means any cross section must have same size than your sources.
I hope I am clear.
If not, just try to move one volume with any translation vector. If the volume is moved, then you have a problem (because it is not connected to the other)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 25, 2013, 10:09
Default
  #3
New Member
 
Jing Shi
Join Date: Feb 2013
Posts: 20
Rep Power: 4
Jing is on a distinguished road
Hi Maxime,

Thank you for your reply. Yes, I have three volumes for three pipes, and the interfaces are connected. When pick a volume, the Cooper is also automatically selected, and with sources (interfaces and the opposite cap )automatically selected too.
But when it is done, the mesh along the axial direction is too sense, which is what I want to change (as is shown in figure). I tried to specify the interval count when mesh the volume, it did not work. No matter which interval count is, it is always the same. Is there a way to specify the mesh density along the axial direction? Say denser near the intersection.

Regards
Jing
Attached Images
File Type: jpg Volume mesh.jpg (82.0 KB, 48 views)
Jing is offline   Reply With Quote

Old   April 25, 2013, 10:23
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
weird...
you can use size function by selecting your source surfaces (meshed) as source and the volume as attachment.
Be sure that the cap face (opposite) isn't mesh (on your picture, it seems you have another meshed volume on the left).
If size function doesn't work, then try to enforce by meshing the cylinder face with map
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 25, 2013, 11:23
Default
  #5
New Member
 
Jing Shi
Join Date: Feb 2013
Posts: 20
Rep Power: 4
Jing is on a distinguished road
Thanks a lot for quick reply. I tried a lot again, still not working...
Yes, in that figure it seems another meshed volume on the left, but the cap face is not meshed before meshing the volume, but once the volume is meshed, it looked like that. Seems that Gambit sweeps the mesh node patterns from the two sides of the pipe even the cap face is not meshed.
I wander is there a way I could spacing an edge along the pipe first. But now there is no edge along the pipe axial direction.

Regards
Jing is offline   Reply With Quote

Old   April 25, 2013, 12:02
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
try this:
delete all volume mesh (with lower geometry enabled)
delete all surface mesh (should be already done, but who knows...)
delete all edge mesh (should be already done, but who knows...)
delete all size functions.
Now
mesh only the 2 surfaces from "interface" (take only one volume)
If it is still not working, share me your dbs file, I will check
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 26, 2013, 05:52
Default
  #7
New Member
 
Jing Shi
Join Date: Feb 2013
Posts: 20
Rep Power: 4
Jing is on a distinguished road
Hi Maxime,

I tried, still not working. Attached is the dbs file, please check. Thank you a lot for your time.

P.s. I drew the cylinder by sweeping along an edge, hoping mesh the edge then could get a meshed volume with the specified interval density along the axial direction. But not working.

Regards
Jing
Attached Files
File Type: zip Tshape.zip (73.7 KB, 22 views)
Jing is offline   Reply With Quote

Old   April 26, 2013, 10:28
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,964
Rep Power: 30
-mAx- will become famous soon enough
ok, it is weird, but I managed myself.
You need to create edges along the cylinder surface. But not as you did, since those edges don't belong to any surfaces.
So:
-delete edge 6
-delete edge 2
-split edge 7 with u-value 0.5 (you get 2 more edges)
-split those 2 edges with also u-value 0.5
-split cylinder surface (6) with vertice 9 and the opposite (on the cap face)
-same with vertice 8
-Now you have both edges on which you can appls and edge mesh as your convenient. Once it is done you can mesh volume

One point more, you need one more split below your "interfaces", in that way you get the 3 volumes.
Sans titre.jpg
Far likes this.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   April 26, 2013, 12:27
Default
  #9
New Member
 
Jing Shi
Join Date: Feb 2013
Posts: 20
Rep Power: 4
Jing is on a distinguished road
Hi Maxime,

Awesome! Following your instruction, finally I know how to make it and have made it.
THANK YOU SO MUCH!

Best Regards,

Jing
Jing 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
how to set periodic boundary conditions Ganesh FLUENT 13 January 22, 2014 05:11
Add Mesh Layers doesnt work on the whole surface Kryo OpenFOAM Native Meshers: snappyHexMesh and Others 8 September 13, 2012 09:28
Mesh elements shape on faces Mohsin FLUENT 3 August 17, 2011 02:37
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 05:18.