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

[ANSYS Meshing] Help mesh a pipe cross

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

Like Tree11Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   December 1, 2012, 13:19
Default Help mesh a pipe cross
  #1
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
Hello everybody,

I'm sorry to post this here, but i've been searching for a while and i can't do this properly. I need to study the flow within a pipe cross like this:

But i can only get this type of mesh, which i believe is not the best one:

I read about blocking and separating the part at the junctions, but i don't know how to do it in desingmodeler.
I also need to do it with three pipes crossing. I really need your help.

Thank you so much in advance!
catrapi is offline   Reply With Quote

Old   December 1, 2012, 14:38
Default
  #2
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
take a look here, hope it can help you
o-grid generation in ANSYS MESHING
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   December 3, 2012, 06:01
Default
  #3
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
Thank you for the answer.

Just another question: So I don't need to divide the geometry in DM because the multizone does that for me? Even if it is a bit more complex than just a simple tube? And is the mesh that I have now, good?

Thank you
catrapi is offline   Reply With Quote

Old   December 3, 2012, 06:04
Default
  #4
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
I found this: http://202.118.250.111:8080/fluent/G...guide/tg03.htm

Should I try and do this in DM?
catrapi is offline   Reply With Quote

Old   December 3, 2012, 13:56
Default
  #5
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,291
Blog Entries: 23
Rep Power: 20
diamondx will become famous soon enough
Quote:
So I don't need to divide the geometry in DM because the multizone does that for me?
Best way to find out is to try, not sure of all the capabilities of Ansys meshing...

About the link you sent me, this is done using Gambit, it can also be done using ICEM CFD.
Start working on that if you want, there are good tutorial and training material that can help do that, it doesn't take too much time... we can assist you too
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   December 5, 2012, 12:07
Default
  #6
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
I've been reading the tutorials and it says that multizone automatically decomposes the geometry. I've tried decomposing myself and it then sweep it, but i found that the elements grew worse than with multizone. So i believe this is the best method.
Thanks diamondx for helping me!
catrapi is offline   Reply With Quote

Old   December 6, 2012, 07:51
Default
  #7
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Lots of slicing in DesignModeler together with Multizone meshing will produce the following. It's faster in ICEM if you know it, otherwise it may be a good choice for you.



Far, RodriguezFatz, Ralen and 1 others like this.
jrunsten is offline   Reply With Quote

Old   December 7, 2012, 05:04
Default
  #8
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
jrunsten, thank you so much!
In fact when I use multiblock, the mesh in the middle becomes triangular
instead of quad. And I read it should be quad in order to get best results. How did you decide where to slice the part? I mean the dimensions? Is it a "more or less like this", or do you have specific places where to slice?

Once again, thank you!
catrapi is offline   Reply With Quote

Old   December 7, 2012, 05:39
Default
  #9
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
This was just some random dimensions i chose, but basically it is all scliced using planes rotated 45 degrees about the origin and then I merged the resulting pieces into the bodies i wanted. Don't forget to create a new part from the final bodies. The only dimension I set for this is the size of the square in the middle.

In ICEM, i guess this would correspond setting the size of the ogrid.

You can my files here:
https://www.dropbox.com/s/butno8c91xeb7hq/cross.wbpz
Maybe it can help someone
jrunsten is offline   Reply With Quote

Old   December 11, 2012, 03:41
Default
  #10
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
@jrunsten Good work. I have two queries:

1. How did you get the hexa meshing at the interface of four pipes (or intersection of two pipes)

2. How to make the wbpz workbench file.
Far is offline   Reply With Quote

Old   December 11, 2012, 03:55
Default
  #11
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Quote:
Originally Posted by Far View Post
@jrunsten Good work. I have two queries:

1. How did you get the hexa meshing at the interface of four pipes (or intersection of two pipes)

2. How to make the wbpz workbench file.
1. It's all in the splits. See the image below. Every part in the multibody cosists of 90 degree bends, making it easy for the Multizone meshing to work



2. In Workbench, choose File>>Archive. The option to restore an archive is directly below.
Far and catrapi like this.
jrunsten is offline   Reply With Quote

Old   December 11, 2012, 04:05
Default
  #12
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
version 14.5 I have 14 so not possible for me to use it (your project uploaded in previous post).
Far is offline   Reply With Quote

Old   December 11, 2012, 04:10
Default
  #13
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Ah ok,

Well I think all the info is here anyway. Perform the slices with your preffered method, create a multibody part and then mesh them all together with a multizone method. For fine grid at the walls, right click the Multizone method and choose "Inflate this method". Choose the correct wall surfaces for each inflation instance and it should work just fine.
jrunsten is offline   Reply With Quote

Old   December 11, 2012, 04:44
Default
  #14
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
Hi, I have version 13, so I'm not able to open.
I tried to split the body, and I can, but I get a lot of parts, and then I'm not able to merge some parts back together (in DesignModeler). Can you please explain to me how you do that?
Thank you!
catrapi is offline   Reply With Quote

Old   December 11, 2012, 04:47
Default
  #15
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Create>>Boolean, Unite
jrunsten is offline   Reply With Quote

Old   December 11, 2012, 05:32
Default
  #16
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
Thank you so much for all your help! I managed to divide it. It took me a while! Thank you
catrapi is offline   Reply With Quote

Old   December 11, 2012, 09:59
Default
  #17
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
Hi,

I don't know if it was posted before, but I can't find it. Is there anyway that I can do a mesh just to one and then replicate it in others? Like if I want these 4 of these crosses connected, can I make a mesh just for the first cross and then make a pattern to mesh the following crosses?
catrapi is offline   Reply With Quote

Old   December 11, 2012, 10:40
Default
  #18
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Not that I'm aware of. You can certainly make a pattern of the geometry in DM, but not in meshing. A bit more work meshing four of them, but not that much.
jrunsten is offline   Reply With Quote

Old   December 11, 2012, 11:10
Default
  #19
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 4
catrapi is on a distinguished road
I did it in DM, but when I try to mesh it, it takes forever, and I end up stoping the mesh... Is there any way I can speed it up?
catrapi is offline   Reply With Quote

Old   December 11, 2012, 11:23
Default
  #20
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 185
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Four in a row or 2x2 like a square?
jrunsten is offline   Reply With Quote

Reply

Tags
ansys meshing, cross, pipe, pipe cross, pipe juction

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
Boundary layer in a pipe Clementhuon OpenFOAM Native Meshers: snappyHexMesh and Others 6 March 12, 2012 13:41
No Surface-Layers on pipe with hexagonal cross sectional area U.Golling OpenFOAM Native Meshers: snappyHexMesh and Others 0 December 10, 2010 10:08
Help needed to generate a graded pipe mesh. jenright OpenFOAM Native Meshers: blockMesh 0 August 22, 2009 08:58
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Terrible Mistake In Fluid Dynamics History Abhi Main CFD Forum 12 July 8, 2002 09:11


All times are GMT -4. The time now is 18:37.