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

[ICEM] Octree not respecting curve parameters

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

Like Tree9Likes
  • 4 Post By PSYMN
  • 4 Post By PSYMN
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   September 30, 2012, 07:35
Default Octree not respecting curve parameters
  #1
siw
Senior Member
 
Join Date: Jul 2009
Posts: 444
Rep Power: 14
siw will become famous soon enough
Hi,

I know that the octree method is patch independent but in the ICEM Help Guide it says that the octree method uses the curve parameters: max size and number of nodes (see image).

I was trying a few things in ICEM today by making a cube and assigning surface and volume sizes for octree. I also assigned a quantity of nodes to one of the cube curves (which would refine the mesh cell at the curve). I ran Build Topology and then ran the octree method but the mesh did not respect the curve nodes. Next I assigned Mesh Curve to the curve with the number of nodes and re-ran octree. But again the mesh did not respect the nodes on the curve.

This must contradict the Help Guide. Or am I missing something?

The reason for trying this is that I need to make a complex hybrid mesh and on some surfaces it would be better to use the autoblock surface method to make structured isotropic and anisotropic quad cells (then split them into tri cells). But on other surfaces I will have to make unstructured tri cells (and the best way to do that is to make an octree volume mesh and delete the volume cells and only the surface cells which will be replaced by the autoblock method - thereby leaving only the unstructured tri cells). Many topics already cover that using octree in this way makes the best quality unstructured surface mesh. So I will need octree to respect the nodes so that the two surface methods are conformal.

Thanks
Attached Images
File Type: jpg Untitled.jpg (86.3 KB, 32 views)
siw is offline   Reply With Quote

Old   October 1, 2012, 10:31
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
The Octree mesher algorithm sees the size on the curves the same way it sees surface sizes. If the size on the curve is smaller than the current octree size, it divides again... In this way, curve sizes can refine octree, but you won't necessarily get the distribution you want.

If you want that sort of control combined with octree you have a few ways to get it...

1) you could start with patch conforming. Make sure the surfaces you want meshed with patch conforming are in different parts from the rest of the surfaces. Mesh those with patch conforming mesh (selected surfaces). Then go to OCtree and use the option for "Use Existing Mesh Parts". You select the parts you already meshed and Compute. Behind the scenes, it will mesh those parts as normal, but then replace the surface mesh with the mesh you already generated and "make consistent" to replace the surface mesh and align the octree volume mesh to it... As a final step, I usually run Delaunay with the TGlib AF option.

2) Knowing what the above does, you could work it out as separate steps. You could mesh your octree tetra as normal, then load the adjacent mesh and merge meshes or Repair => make consistent. Again, part assignment (distinction) is important for selecting where the mesh is aligned.
Far, siw, cfd seeker and 1 others 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   October 1, 2012, 10:32
Default
  #3
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
Oh yea, I will get them to fix that incorrect doc...

Thanks for pointing it out.
__________________
-----------------------------------------
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   October 1, 2012, 14:48
Default
  #4
siw
Senior Member
 
Join Date: Jul 2009
Posts: 444
Rep Power: 14
siw will become famous soon enough
Thanks for the information Simon, yep that table in the Help Guide gave me the wrong idea of what happens. You should document all this useful knowledge in an ICEM guide annex since the Help Guide lacks so much detail compared with the other ANSYS documents.

I'll give these a try but I have found that the patch conforming surface mesher fails on the simplest of shapes - such as a hemisphere surface for an external aero farfield boundary. Even though the geometry is water-tight and Build Topo is good.

Otherwise, it's back the ever futile attempts at hexa blocking. I lost my weekend in the office trying to block this geometry and ended up on sunday evening at the same place I was on saturday morning.
siw is offline   Reply With Quote

Old   October 1, 2012, 16:12
Default
  #5
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 helps to understand how each algorithm works (explanations are provided under the theory sections of the doc)...

The patch conforming algorithm starts by extracting loops from each surface (or group of surfaces) and then it seeds the perimeter with the curve node spacing.

Then it meshes the perimeter with line elements.

Then it uses a recursive loop paving algorithm, projected to surface, to lay out the shell elements.

If you have something like a hemisphere or seamless cylinder, it can't really figure out the projection or edge sizing (respectively). The fix is to subdivide the curved shapes using tools provided under geometry => Repair. Once subdivided, patch conforming should have no trouble meshing those shapes.
Far, siw, BrolY and 1 others 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   October 1, 2012, 22:59
Default
  #6
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:
You could mesh your octree tetra as normal, then load the adjacent mesh and merge meshes or Repair => make consistent.
By load, you mean meshing the surface a part, save it in a mesh file. and mesh the other part, open the saved mesh, select merge, then do the repair ? it's sounds like a boolean operation ! am i right ?
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   October 1, 2012, 23:07
Default
  #7
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:
I lost my weekend in the office trying to block this geometry and ended up on sunday evening at the same place I was on saturday morning.
I smiled when i read this.
I felt happy because i was like "oh i'm not the only one"
I know exactly how you feel and it just happened to me too this week end.
Good luck...
If it's not confidential, i'm curious to know how it looks like, may be some of us can give you a blocking strategy ?
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   October 2, 2012, 10:19
Default
  #8
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
Quote:
it's sounds like a boolean operation ! am i right ?
A boolean operation is when you add two volumes or subtract one from another. With most geometry or meshing tools, this is really talking about changing the definition of the body, rather than just sitting two bodies next to each other.

Usually, users are asking how to subtract one volume from another so they can mesh the new region defined by the space between the bodies. In ICEM CFD, we just place a material point between the volumes and flood fill. We don't change (or even recognize) the body definitions.

In this particular case, we are just talking about meshing two volumes separately and then then merging the mesh on the shared face. No volumes were "unioned" or anything like that. We just made the nodes line up and then merged them.
__________________
-----------------------------------------
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   October 2, 2012, 11:26
Default
  #9
Senior Member
 
Join Date: Mar 2011
Location: Germany
Posts: 414
Rep Power: 11
cfd seeker is on a distinguished road
Quote:
you could start with patch conforming. Make sure the surfaces you want meshed with patch conforming are in different parts from the rest of the surfaces. Mesh those with patch conforming mesh (selected surfaces). Then go to OCtree and use the option for "Use Existing Mesh Parts". You select the parts you already meshed and Compute. Behind the scenes, it will mesh those parts as normal, but then replace the surface mesh with the mesh you already generated and "make consistent" to replace the surface mesh and align the octree volume mesh to it... As a final step, I usually run Delaunay with the TGlib AF option.
So by this way tetra will take sizes from the curves and these curve parameters will be fallowed all along the surface b/w the two curves isn't it?
cfd seeker is offline   Reply With Quote

Old   October 2, 2012, 12:39
Default
  #10
siw
Senior Member
 
Join Date: Jul 2009
Posts: 444
Rep Power: 14
siw will become famous soon enough
diamondx,

no I cannot show the model as it is commerically sensitive. So I have to use generic examples (such as Far's 1/4 missile topic) to get assistance with my model when asking questions here.
siw is offline   Reply With Quote

Old   October 2, 2012, 16:24
Default
  #11
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
@CFD Seeker...

No, I wouldn't say that tetra takes the curve distributions... The patch conforming surface mesher does... Then we make the tetras conformal to that... But yes, in the end, you have a tetra/tri mesh that lines up with your specified curve node distribution...
__________________
-----------------------------------------
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   October 3, 2012, 03:46
Default
  #12
siw
Senior Member
 
Join Date: Jul 2009
Posts: 444
Rep Power: 14
siw will become famous soon enough
To get the patch conforming tri cells to respect the nodes in a curve do we need to use the Mesh > Mesh Curve at all?

Also, the smoothing of the patch conforming surface elements detaches them from the nodes (note: I don't smooth the adjacent autoblock surface mesh). How can the node conformance be fixed during smoothing?

Thanks
Attached Images
File Type: jpg Untitled.jpg (35.0 KB, 4 views)

Last edited by siw; October 3, 2012 at 03:53. Reason: typo
siw is offline   Reply With Quote

Old   October 3, 2012, 09:58
Default
  #13
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
@SIW

No, you don't need to use the curve meshing option unless you only want to mesh the curves (this happens a lot in the FEA world. For instance, they may want to simulate the fluid flow by placing a curve down the middle of a pipe and generating elements on it... They tie those in to the surrounding FEA mesh as a sort of connected 1D CFD component to improve the accuracy of the cooling...)

If you want to keep a particular distribution while smoothing, you can control it at the smoother by freezing triangles or a particular part or subset. Or you could go into move nodes => Lock Elements. You could lock triangles or just the line elements between the nodes. Note that for some reason, a node is only locked if you choose the line element on both sides of it.
siw likes 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

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
Pro/E to ANSYS Parameterization Guide Trues ANSYS 1 September 21, 2012 10:05
block-structured mesh for t-junction Robert@cfd ANSYS Meshing & Geometry 20 November 11, 2011 05:59
[ICEM] Problems with coedge curves and surfaces tommymoose ANSYS Meshing & Geometry 0 August 5, 2011 16:02
How to maintain spacing along a new curve? KB Main CFD Forum 2 June 5, 2007 16:45
CFX4.3 -build analysis form Chie Min CFX 5 July 12, 2001 23:19


All times are GMT -4. The time now is 05:29.