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

[ICEM] beautiful o-grid

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

Like Tree1Likes
  • 1 Post By diamondx

Reply
 
LinkBack Thread Tools Display Modes
Old   January 22, 2013, 13:07
Default beautiful o-grid
  #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
dear Icemers ,

i have a problem, please refer to the picture below



when i need to make a blocking for a circle, and after doing the splits, the associations always come up with this kind of grid. How can i obtain straight and neat square inside the circle since it plays very much on the quality later. Is there a way for doing that ??

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

Old   January 22, 2013, 17:48
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
ok problem solved never mind...
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali

Last edited by diamondx; January 22, 2013 at 19:12.
diamondx is offline   Reply With Quote

Old   January 22, 2013, 18:07
Default
  #3
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
how?...........
Far is offline   Reply With Quote

Old   January 22, 2013, 18:36
Default
  #4
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
sorry for giving fake hope. but i solved the problem but changing my blocking strategy...
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   January 22, 2013, 19:25
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
Let me share what i have done so far. my initial geometry was a cylinder, with a series of holes around it. blocking is doable, but you have to be very careful to the location of vertex etc... another way of doing this is to block a portion of the cylinder and rotate the mesh. as the picture shows, i took just a small portion of the cylinder and meshed it:



quality is good enough, min angle too, but i just don't like the stretched element near the edge, what do you guys think of this blocking , i can share the project if you want.
davidwilcox likes this.
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   January 23, 2013, 05:57
Default
  #6
Senior Member
 
Christoph
Join Date: May 2011
Location: Germany
Posts: 182
Rep Power: 9
energy382 is on a distinguished road
Quote:
Originally Posted by diamondx View Post
Let me share what i have done so far. my initial geometry was a cylinder, with a series of holes around it. blocking is doable, but you have to be very careful to the location of vertex etc... another way of doing this is to block a portion of the cylinder and rotate the mesh. as the picture shows, i took just a small portion of the cylinder and meshed it:



quality is good enough, min angle too, but i just don't like the stretched element near the edge, what do you guys think of this blocking , i can share the project if you want.
That's ok. I recently had a centrifugal pump simulation with a heavy curved blade, so my inflow/inlet looks similar (or to be precise: much more curved).
Look at your min. ortho, max. dehedral and your volume change. These paramters are much more important than deter. or angle in my experience.

I often had meshes with a lower angle, but good ortho and they achieved better and faster solution than good angles and bad ortho.
energy382 is offline   Reply With Quote

Old   January 23, 2013, 06:32
Default
  #7
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
From my point of view, you reached the limit of structured mesh done with blocking Some areas are over-refined, but you can't avoid it.

About the quality values, it would depend a lot on your solver. For some of them, min angle is very important, and for others, it's not a top priority criterion.

About your blocking, I think you could move some vertices to improve the nodes repartition and maybe add some elements to have a better volume change. Otherwise, your strategy looks good !
BrolY is offline   Reply With Quote

Old   February 7, 2013, 15:27
Default
  #8
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'm back dear friend,

I have a question about these criterion: max dihedral and volume change. from your experience what is the range of acceptable values. what i found so far is that it should be 10<x<170 for the max dihedral. i couldn't find any for the volume change...

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

Old   February 7, 2013, 17:23
Default
  #9
Senior Member
 
Christoph
Join Date: May 2011
Location: Germany
Posts: 182
Rep Power: 9
energy382 is on a distinguished road
Quote:
Originally Posted by diamondx View Post
i'm back dear friend,

I have a question about these criterion: max dihedral and volume change. from your experience what is the range of acceptable values. what i found so far is that it should be 10<x<170 for the max dihedral. i couldn't find any for the volume change...

thanks a lot
You've to be carefull about the volume change. Once, I made a mesh study (turbine blade) and had just one block, were I've forgotten to adjust spacing 1 (and therefore had volume change of 170).
The mesh achvied a very good convergence (max Res <10E-4), but produced physically invalid results!
A good value is <5, but <10 is also acceptable.

Just make a best practice with three meshes (global scale factor arround 0.7 and 1.4). and create some monitor points (e.g. pressure difference...). These values should either fall constantly from coarse to fine (mesh) or go up. If so, your mesh is fine. If not, you've to look about your volume change, orthogonality etc...
energy382 is offline   Reply With Quote

Old   February 8, 2013, 14:25
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
christoph, thanks a lot for you answer.
there was a major change in the geometry, and it turns out i had to use a quarter of the cylinder because more holes were added
However, as shown below, the holes gave me hard time to block. i spent the hole day yesterday trying to get a descent blocking.




having to add an o-grid for all the holes, and because it's cylindrical, the move vertices can't be applied as i can't fix the x or y or z.
i just don't know how to deal with them, is there some kind of automatic arrangement to deal with these o-grid ?? i'm asking for too much



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

Old   February 8, 2013, 14:45
Default
  #11
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:
Originally Posted by diamondx View Post

having to add an o-grid for all the holes, and because it's cylindrical, the move vertices can't be applied as i can't fix the x or y or z.
thats why I asked for this feature
New Feature in ICEM is required
Far is offline   Reply With Quote

Old   February 8, 2013, 14:54
Default
  #12
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 voted for it

I started to hate perforated cylinders like these, i guess i should go unstructured...
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   February 9, 2013, 07:36
Default
  #13
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:
Originally Posted by energy382 View Post
You've to be carefull about the volume change. Once, I made a mesh study (turbine blade) and had just one block, were I've forgotten to adjust spacing 1 (and therefore had volume change of 170).
The mesh achvied a very good convergence (max Res <10E-4), but produced physically invalid results!
A good value is <5, but <10 is also acceptable.

Just make a best practice with three meshes (global scale factor arround 0.7 and 1.4). and create some monitor points (e.g. pressure difference...). These values should either fall constantly from coarse to fine (mesh) or go up. If so, your mesh is fine. If not, you've to look about your volume change, orthogonality etc...
Good info. This may be important and manageable in internal flows but impossible to keep in external aero CFD. When downstream domain extent may be stream-wise : 15 upstream and 20-30 downstream. Transverse may be up to 15-20 lengths.

More it is important in the critical flow areas (external flows) near wall or it is necessary to keep the volume change <10 in farfield?

Can we use the global scale factor for Hexa? when combined with part mesh setup and update all option we can use it but how to define the local spacing and growth ratio? Manually?
Far is offline   Reply With Quote

Old   February 11, 2013, 03:54
Default
  #14
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
You can move vertices by fixing a direction, which is very useful for o-grid. It requires times, but at the end, you can place the vertice wherever you want.
Otherwise, align vertices in line tool is very useful too.

About the volume change, I would say the first limit is your number of elements. For industrial cases, and especially when dealing with hexa, you can't increase too much the number of elements .. Anyway, I think < 20 is ok, and < 10 is good !
BrolY 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
MapFields to New Grid For Extreme Grid Deformations due to Body Motion albcem OpenFOAM 0 May 5, 2009 14:17
Grid Adaptation Suresh FLUENT 0 October 15, 2003 13:18
GRID TO GRID INTERPOLATION in FLUENT calogero FLUENT 3 June 4, 2003 08:32
Combustion Convergence problems Art Stretton Phoenics 5 April 2, 2002 05:59
Troubles modelling flow through a grid Hans Klaufus CFX 1 June 28, 2000 16:43


All times are GMT -4. The time now is 09:14.