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

[ANSYS Meshing] o-grid generation in ANSYS MESHING

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

Like Tree16Likes
  • 3 Post By diamondx
  • 2 Post By PSYMN
  • 2 Post By PSYMN
  • 3 Post By diamondx
  • 6 Post By diamondx

Reply
 
LinkBack Thread Tools Display Modes
Old   September 11, 2012, 10:14
Default o-grid generation in ANSYS MESHING
  #1
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
I wanna generate a structured mesh in a tube using ANSYS MESHING.
Using the sweep method or Multizone.
for an o-grid, i need to slice the geometry following the picture below:


How to slice it like that. do i need to go back to designmodeler, and create the square in the middle with the edges then go back to the meshing software ?
Is there another way for that ?

Thanks !!
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 12, 2012, 09:01
Default
  #2
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
In ANSYS Meshing, MultiZone figures out the volume subdivision for you...

It just needs you to ask for Inflation layers.

After setting up the MultiZone method...

Left Click on the Mesh Branch to view its Details Panel...

Under "Inflation", set "Use Automatic Inflation" as "Program Controlled"...

This option basically just assumes that you don't want Named Selections inflated (Not INLET, OUTLET, SYMMETRY, etc.) and that most people don't bother putting their walls in Named selections... It works for me because I have the flat ends as my inlet and outlet. If you have a named selection or some other way you want to select the surfaces to be inflated, you can choose "All Faces In a Named Selection". Unfortunately, you can not use "Insert => Inflation" with Multizone because it requires a global definition.

AMESH_OGRID.jpg

One other catch, if your mesh comes out looking swept, you just need to take better control over the mapping using some of the multizone controls...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   September 12, 2012, 12:17
Default
  #3
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
Thanks Simon for your reply.
I had to add the mapped face meshing and select the inlet and outlet to get the same elements as yours. below are the some screenshots with and without the face mapped meshing.


Without face mapped meshing:



May be because of length of the tubes ??? I have one more question, I have version 13, and i just got into ansys meshing, when i tried to get like your mesh, i tought that maybe it's because you have version 14. so i tried it on another pc here in the lab , result was same, but i got into one interesting feature which is the ICEM CFD override , i tried that and i discovered that i can actually mesh it in icem interactively... that was just amazing... so i also discovered that i can create material bodies like in ICEM CFD. that means i don't have to extract an volume of fluid...

If this tube is inside a complicated heat exchanger for example (Because i'm working on one actually), i can combine a hexa mesh in the tube (blocked with icem) and a tetra mesh using material point in ansys meshing... it's something that ICEM CFD CAN'T DO (unless you use non-condormal mesh). are my assumptions correct ? this is what i was trying to do yesterday in icem without successful result even with multizone. So may be it's more easy with ansys meshing ?

Thanks a lot for you answers...
Far, FJSJ and Asura like this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 12, 2012, 12:40
Default
  #4
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
It is easy to go from ANSYS Meshing to ICEM CFD... The trick is getting back again. ANSYS Meshing is really picky about the geometry and mesh connection. If you change any of the geometry in ICEM CFD (part names, add a curve, anything), the mesh will not go back...

This option to mesh in ICEM CFD gets better every release. 14.5 is much better than 13.0.


In ANSYS Meshing, you can not combine the concepts of "Assembly Meshing" which uses a material point, and Part by Part meshing methods like MultiZone.

However, we are working on a way to have assembly meshing (material point PI meshing) within specified Mulizone Blocks... Which will be very cool.

In ICEM CFD, you can do this sort of thing, but you need to use "merge mesh".

Many people just use a non conformal mesh and join things in the solver.
Far and chienfm like this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   September 12, 2012, 12:56
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
Ok... Until then i'll choose what's best for me.
still it's great to have this interoperability...
Thanks, thanks a lot.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 12, 2012, 13:00
Default
  #6
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
Blog Entries: 6
Rep Power: 38
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Your comments are worth reading the help files ten times.

Quote:
Originally Posted by PSYMN View Post
It is easy to go from ANSYS Meshing to ICEM CFD... The trick is getting back again. ANSYS Meshing is really picky about the geometry and mesh connection. If you change any of the geometry in ICEM CFD (part names, add a curve, anything), the mesh will not go back...

This option to mesh in ICEM CFD gets better every release. 14.5 is much better than 13.0.


In ANSYS Meshing, you can not combine the concepts of "Assembly Meshing" which uses a material point, and Part by Part meshing methods like MultiZone.

However, we are working on a way to have assembly meshing (material point PI meshing) within specified Mulizone Blocks... Which will be very cool.

In ICEM CFD, you can do this sort of thing, but you need to use "merge mesh".

Many people just use a non conformal mesh and join things in the solver.
Far is offline   Reply With Quote

Old   September 12, 2012, 16:23
Default
  #7
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
@Far...

Except that I often help the doc team write the Help files
Far and yashganatra like this.
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   September 14, 2012, 03:18
Thumbs up
  #8
Member
 
Hugh Ingham
Join Date: Aug 2012
Posts: 35
Rep Power: 4
martyn88 is on a distinguished road
Hi Psymn and diamondx. I have a problem that is similar to that explained by diamondx. I wish to create a structured grid for use in a LES simulation.

However my geometry is slightly more complicated than a simple pipe. My domain is a converging-diverging nozzle surrounded by ambient fluid (see below pictures):

meshpic.jpg

I really can't afford to model the entire geometry so I am hoping to only model a section (1/8 or 1/4) with periodic side boundaries.

Originally I swept a 2-D grid through the wedge but the cells near the centreline were tet prisms with very high aspect ratio, and were affecting my solution. Therefore I need to use an O-grid.

I tried following your steps above but ran into some problems when trying to mesh the wedge region:

mesho_grid.jpg


Is there a way of creating a more symmetrical mesh on the wedge face? Also what is the best way to refine it? Can I specify edge sizings?

Thanks,

Hugh
martyn88 is offline   Reply With Quote

Old   September 14, 2012, 09:04
Default
  #9
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
You can select any geometry edge, right click => Insert => Sizing. You can set the element size or you can set a "number of divisions" with a bias, etc.

For something like a 30 degree wedge, MultiZone doesn't really give you a way to create a quarter OGrid automatically. You could go to ICEM CFD and mesh this model with all the control you could ever want (and some learning curve) or you could figure out how to slice the model in DM...

Sorry, I am not really very expert at slicing in DM and don't have time to try it out to be sure I am giving you the right info ;^)
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey

Last edited by PSYMN; September 14, 2012 at 10:48. Reason: clarify
PSYMN is offline   Reply With Quote

Old   September 14, 2012, 09:27
Default
  #10
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
there you go, made in Icem:

Here is the project file:
https://dl.dropbox.com/u/35161486/LES.zip
Far, PSYMN and chienfm like this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 14, 2012, 09:37
Default
  #11
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
Here is a small video on how to do that :
http://youtu.be/InyeCmEuUVM
Far, PSYMN, stuart23 and 3 others like this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 14, 2012, 13:54
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
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:
Originally Posted by diamondx View Post
there you go, made in Icem:

Here is the project file:
https://dl.dropbox.com/u/35161486/LES.zip
similar thread LES mesh
Far is offline   Reply With Quote

Old   September 16, 2012, 05:23
Default
  #13
Member
 
Hugh Ingham
Join Date: Aug 2012
Posts: 35
Rep Power: 4
martyn88 is on a distinguished road
Wow thankyou so much Ali, you have been a massive help! I will have a play around in ICEM tomorrow and try and get my head around it. You have given me a big head start though
Really appreciate it.

Hugh
martyn88 is offline   Reply With Quote

Old   September 20, 2012, 16:57
Default
  #14
Senior Member
 
PSYMN's Avatar
 
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,662
Blog Entries: 1
Rep Power: 35
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hey DiamondX, FAR or anyone else who wants to make a video...

If you would like to share it with a larger audience, please email your youtu.be link to "social@ansys.com" and tell them they are welcome to post it in the user generated content area of the ANSYS youtube site. If it is a technical demo, ask them to put it under tech tips. ANSYS can hit the "like" button and add it to their favorites so it shows up on the ANSYS channel. Of course, there is no guarantee they will like your video ;^).

One other thing, please make sure that the description of your video clearly states what the demo shows so that people can find the right ones...
__________________
-----------------------------------------
Please help guide development at ANSYS by filling in these surveys

Public ANSYS ICEM CFD Users Survey

This second one is more general (Gambit, TGrid and ANSYS Meshing users welcome)...

CFD Online Users Survey
PSYMN is offline   Reply With Quote

Old   September 21, 2012, 01:33
Default
  #15
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,914
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:
Originally Posted by PSYMN View Post
Hey DiamondX, FAR or anyone else who wants to make a video...

If you would like to share it with a larger audience, please email your youtu.be link to "social@ansys.com" and tell them they are welcome to post it in the user generated content area of the ANSYS youtube site. If it is a technical demo, ask them to put it under tech tips. ANSYS can hit the "like" button and add it to their favorites so it shows up on the ANSYS channel. Of course, there is no guarantee they will like your video ;^).

One other thing, please make sure that the description of your video clearly states what the demo shows so that people can find the right ones...
Fantastic.
Far is offline   Reply With Quote

Reply

Tags
ansys meshing, blocking strategy, o-grid generation, structured mesh

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
[ANSYS Meshing] Meshing a t-pipe in Ansys Meshing Kirjain ANSYS Meshing & Geometry 6 August 15, 2012 02:03
How To save a created mesh file in Ansys Meshing ashtonJ CFX 4 January 7, 2012 23:04
Hexa Block meshes in ANSYS Meshing? siw ANSYS Meshing & Geometry 3 July 31, 2009 10:40
structured grid generation pertup Main CFD Forum 0 November 2, 2004 04:05
Help Re. Grid Generation Patel Amit R. FLUENT 1 February 28, 2003 22:27


All times are GMT -4. The time now is 21:53.