|
[Sponsors] |
[ICEM] Octree not respecting curve parameters |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 30, 2012, 07:35 |
Octree not respecting curve parameters
|
#1 |
Senior Member
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25 |
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 |
|
October 1, 2012, 10:31 |
|
#2 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
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.
__________________
----------------------------------------- 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 |
|
October 1, 2012, 10:32 |
|
#3 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
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 |
|
October 1, 2012, 14:48 |
|
#4 |
Senior Member
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25 |
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. |
|
October 1, 2012, 16:12 |
|
#5 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
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.
__________________
----------------------------------------- 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 |
|
October 1, 2012, 22:59 |
|
#6 | |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
Quote:
|
||
October 1, 2012, 23:07 |
|
#7 | |
Super Moderator
Ghazlani M. Ali
Join Date: May 2011
Location: Tokyo, Japan
Posts: 1,385
Blog Entries: 23
Rep Power: 28 |
Quote:
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 ? |
||
October 2, 2012, 10:19 |
|
#8 | |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
Quote:
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 |
||
October 2, 2012, 11:26 |
|
#9 | |
Senior Member
Join Date: Mar 2011
Location: Germany
Posts: 552
Rep Power: 20 |
Quote:
|
||
October 2, 2012, 12:39 |
|
#10 |
Senior Member
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25 |
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. |
|
October 2, 2012, 16:24 |
|
#11 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
@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 |
|
October 3, 2012, 03:46 |
|
#12 |
Senior Member
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 733
Rep Power: 25 |
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 Last edited by siw; October 3, 2012 at 03:53. Reason: typo |
|
October 3, 2012, 09:58 |
|
#13 |
Senior Member
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,663
Blog Entries: 1
Rep Power: 47 |
@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.
__________________
----------------------------------------- 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 |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ICEM] Problems with coedge curves and surfaces | tommymoose | ANSYS Meshing & Geometry | 6 | December 1, 2020 11:12 |
Pro/E to ANSYS Parameterization Guide | Trues | ANSYS | 4 | April 18, 2018 05:52 |
block-structured mesh for t-junction | Robert@cfd | ANSYS Meshing & Geometry | 20 | November 11, 2011 04:59 |
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 |