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 11, 2012, 10:26
Default
  #21
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
I'm doing 4 in a row! I'm trying to model a scaffold structure.

PS - I cannot thank you enough for helping me!
catrapi is offline   Reply With Quote

Old   December 11, 2012, 14:59
Default
  #22
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
Hi,

After battling with this for a while, I figured it out that I couldn't do this with Multiblock Meshing. So I setted the dimesions and used the automatic method. I got the following:



The problem is that I don't get Hexa meshing everywhere. And I get a warning for mesh skewness bigger than 0.98...
catrapi is offline   Reply With Quote

Old   December 12, 2012, 05:33
Default
  #23
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 166
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
The order in which you mesh the bodies are important when the geomtries get complicated. My guess is that the "core" of the pipe is meshed in a nice H-grid fashion first, which makes the 90 degree bends impossible to sweep with the multizone method. If you look at the images below, the way the core is meshed affects the outer bodies:




Also, by just hitting "Generate Mesh" you are giving Ansys one hell of a challenge here. What I do is to first hide all the core bodies, then mesh some of the outer bodies in steps. Start with just one by selecting the body, right click and choose "Generate Mesh on Selected bodies".



Then you can select the remaining bodies in that cross and mesh them together, followed by one cross at a time. So in total 5 steps.
When you have all the outer bodies meshed, go ahead and do the inner ones as well.

ALSO, looking at your images, it seems that you dont have node matching between the different crosses. Make sure that you create ONE part in DM after you have created your pattern.

Far, ghost82 and chienfm like this.
jrunsten is offline   Reply With Quote

Old   December 12, 2012, 05:38
Default
  #24
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,876
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Great work.

Btw this would be much easier in ICEM right?
Far is offline   Reply With Quote

Old   December 12, 2012, 05:41
Default
  #25
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
jrunsten, I can't thank you enough! I didn't know that the mesh had to be generated step by step! Thank you for going through so much trouble to help me! I will try it now!
catrapi is offline   Reply With Quote

Old   December 12, 2012, 05:43
Default
  #26
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 166
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
Quote:
Originally Posted by Far View Post
Great work.

Btw this would be much easier in ICEM right?
Thanks, nice practice for me also

Yes, ICEM would be easier (you should know ), and is where I would do it if I were to choose. But I like to use the Ansys tools as well and see how well they can compete.

But for just one project, with no previous experience in either tool, I'm not sure the time it would take to get into the ICEM way of thinking is worth it?
jrunsten is offline   Reply With Quote

Old   December 12, 2012, 05:52
Default
  #27
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,876
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by jrunsten View Post
Thanks, nice practice for me also

Yes, ICEM would be easier (you should know ), and is where I would do it if I were to choose. But I like to use the Ansys tools as well and see how well they can compete.

But for just one project, with no previous experience in either tool, I'm not sure the time it would take to get into the ICEM way of thinking is worth it?

hahaha. I know the ICEM and it is relatively easy (some times I also feel helpless ) for me now to work with ICEM. ICEM is not a straight forward way of thinking and it is combination of ICEM and user which makes it work so powerfully. So human is always there in ICEM to use its full power.

On the other hand Ansys has tried to make the Ansys meshing automatic, accurate, easy to make models and easy to learn. But I am just amazed by its power as you have shown to us. Really impressed. In my understand the method you are using is also considered advance level method in AM too.

But you are right for one project it is better to go for the easy option if it does the job.

You are also giving me inspiration that I should also get my hands dirty with AM and DM thoroughly.
Far is offline   Reply With Quote

Old   December 12, 2012, 07:21
Default
  #28
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
OK, It's driving me crazy! I followed everyone of your steps, and I can't mesh it! Did you use multiblock? I get the error that the geometry can't be sweeped. Then I tried other methods and the geometry gets a triangular mesh. I really don't know what's the problem! I feel like a retard!
catrapi is offline   Reply With Quote

Old   December 12, 2012, 08:07
Default
  #29
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 166
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
If you upload an archive of the project I can take a look later
jrunsten is offline   Reply With Quote

Old   December 12, 2012, 08:59
Default
  #30
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
My files are here: https://dl.dropbox.com/u/3548610/Circ.UC.G1.1p0.yz.wbpz

Thank you so much!
catrapi is offline   Reply With Quote

Old   December 14, 2012, 06:27
Default
  #31
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
Hello. I don't want to be a nag, but did you figure something out? I'm trying, but I always get the same result.
catrapi is offline   Reply With Quote

Old   December 14, 2012, 06:34
Default
  #32
Senior Member
 
Josef Runsten
Join Date: Jul 2010
Location: Gothenburg, Sweden
Posts: 166
Rep Power: 13
jrunsten will become famous soon enough
Send a message via MSN to jrunsten
I opened and tried really fast but I also had errors. Won't have time to look more into it today at least, but I am interested in what the problem is, so maybe I'll have a go in the weekend. You know, for fun.
jrunsten is offline   Reply With Quote

Old   December 14, 2012, 08:30
Default
  #33
Senior Member
 
Christoph
Join Date: May 2011
Location: Germany
Posts: 182
Rep Power: 8
energy382 is on a distinguished road
this topology is meshed in icem hexa within 5min or less. so why do you go for ansys meshing tool?!
energy382 is offline   Reply With Quote

Old   December 14, 2012, 09:12
Default
  #34
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
I have to get this done by this weekend. I don't think I have time to learn how to use ICEM properly... :/
catrapi is offline   Reply With Quote

Old   December 14, 2012, 09:26
Default
  #35
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,876
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Meshing one pipe or several pipes will take the same time in ICEM Five minutes

You can learn ICEM within 10 minutes
Attached Images
File Type: jpg pipe001.jpg (41.7 KB, 40 views)
File Type: jpg pipe002.jpg (46.6 KB, 44 views)
File Type: jpg pipe003.jpg (73.9 KB, 40 views)
File Type: jpg pipe005.jpg (48.8 KB, 43 views)
Attached Files
File Type: zip pipe.zip (41.6 KB, 9 views)
jrunsten likes this.

Last edited by Far; December 14, 2012 at 09:43.
Far is offline   Reply With Quote

Old   December 14, 2012, 10:33
Default
  #36
Super Moderator
 
diamondx's Avatar
 
Ghazlani M. Ali
Join Date: May 2011
Location: Canada
Posts: 1,216
Blog Entries: 22
Rep Power: 18
diamondx will become famous soon enough
Send a message via MSN to diamondx
In ICEM , you can then you duplicate or copy the mesh without meshing everything
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is online now   Reply With Quote

Old   December 14, 2012, 10:36
Default
  #37
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,876
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by diamondx View Post
In ICEM , you can then you duplicate or copy the mesh without meshing everything
Hey we are here not to kill Ansys meshing
Far is offline   Reply With Quote

Old   December 14, 2012, 10:44
Default
  #38
New Member
 
Join Date: Nov 2012
Posts: 20
Rep Power: 3
catrapi is on a distinguished road
Thank you all. I'm going to give it a go in ICEM then!
PS- Thank you for the files Far
catrapi is offline   Reply With Quote

Old   December 14, 2012, 11:02
Default
  #39
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,876
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Important tips

1. Use the clean geometry (without slices made in DM)
2. Build topology
3. use two splits horizonality and two vertically (assuming you have two pipe in cross). If there are more pipes in series, increase the vertical splits
4. Delete unwanted blocks
5. Associate edge to curves on the ends of each pipe. For simple case i.e. two pipes intersecting, you have four ends.
6. Important Associate two vertices to each intersecting curves at intersection of two pipes. You have total 8 vertices and four curves.
7. Go to O-grid panel and then select all blocking and faces at each end of pipes and apply
8. Set mesh parameters
9. Select solver
9. Set boundary conditions
10. Output mesh.
11. Import into Fluent.
chienfm likes this.
Far 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 09:08
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 14:52.