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

[ICEM] Shell Patch Dependent method query

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

Like Tree2Likes
  • 1 Post By PSYMN
  • 1 Post By PSYMN

Reply
 
LinkBack Thread Tools Display Modes
Old   November 18, 2009, 13:14
Default [ICEM] Shell Patch Dependent method query
  #1
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
Hi,

I'd like to know how this method works. The help manual says that loops are closed regions made by curves or surfaces and the mesh is seeded according to the curve node spacing.

So if I've got a closed region made of curves with node spacings how does the seeding work? And once the shell is seeded does it use the delaunay triangulation to join the nodes to make the elements? And what does it do if during the delaunay stage it needs to modify the seeded nodes.

Or is there a tech paper that I can get that will tell me what/how ICEM is using/doing.

Thanks.
siw is offline   Reply With Quote

Old   November 19, 2009, 12:56
Default Papers
  #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
For now, here are some papers, but I will come back when I have some time and describe the process in English...

Kolms, A.: On Automatic Generation of Quadrilateral Surface Meshes. ZAMM 76 (1996) S5 261-262

Sluiter, M. L. C.; Hansen, D. L.: A general purpose automatic mesh generator for shell and solid finite elements. Computers in Engineering 3 (1982) 29-34



Talbert, J. A.; Parkinson, A. R.: Development of an automatic two-dimensional finite element mesh generator using quadrilateral elements and Bezier curve boundary conditions. Int. J. for Numer. Methods Eng. 29 (1990) 1551-1567
PSYMN is offline   Reply With Quote

Old   November 20, 2009, 10:21
Default
  #3
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
Appreciated, thanks.

I'm using the patch dependent with the all tri element type for the mesh in my research and would need to write a bit about the meshing in the thesis, so the info will be useful.
siw is offline   Reply With Quote

Old   August 22, 2013, 13:02
Default
  #4
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Hi all,

Anybody can help me what are the differences/advantages of patch dependent over patch independent ?

Thanks in advance
Amir1 is offline   Reply With Quote

Old   August 26, 2013, 11:37
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
Quote:
Originally Posted by Amir1 View Post
Hi all,

Anybody can help me what are the differences/advantages of patch dependent over patch independent ?

Thanks in advance
Patch dependent (aka patch conforming) is faster and often gives a much nicer looking or even mapped mesh, especially if the sizing function is designed for it (such as with Gambit, ANSYS Meshing or Fluent Meshing). ICEM CFD meshing also has a patch dependent method, but it does not work with our sizing function, so you need to set the edge distributions explicitly. Patch dependent methods usually allow for "hard" sizing where you can set the exact number of nodes you want on any edge. Patch dependent is also constrained by the surface patches (problem if you have slivers or gaps) and requires a nice water tight model (either at the geometry stage or you need to fix up the surface mesh afterward) before you can proceed to a volume method.

The Patch independent method takes longer, but it gives you the volume mesh at the same time. Patch independent methods are not concerned about surface topology, small gaps, etc, so they are much more robust. They are also more robust because you don't have to worry about the delaunay or advancing front failures when you generate your volume mesh. Patch independent methods do not give the nice mapped mesh on fillets (unless you guide them with isoparametric curves). Since parch independent methods do not start from the edges, they often rely on "SOFT" sizing that does not necessarily respect the number of nodes you set on an edge. Octree methods typically only allow step changes in the mesh size and will round down any other sizes set.

Anyone else want to comment?
__________________
-----------------------------------------
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   August 27, 2013, 16:52
Default
  #6
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Thanks for your response.

I have been trying to creat a good mesh in ICEM but now facing with lots of difficulties. Can you please help me how to fix them?

I m trying to creata mesh in a box which consist of three cylinders such a way that two straght plate are passting through them.

So at the regions where strips contact the rolls there are some error.

I have tried CHECK MESH and SMOOTH MESH and Check Quality.
None of the worked.
I really dont know what do?

Please help me

Thanks,
Amir
Amir1 is offline   Reply With Quote

Old   August 27, 2013, 17:03
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
@Amir1...

What is the error? Can you show some screen shots of the problem areas?
__________________
-----------------------------------------
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   August 27, 2013, 17:20
Default
  #8
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
I m trying to upload the photos but the website supports only small images.
Amir1 is offline   Reply With Quote

Old   August 27, 2013, 17:36
Default
  #9
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Hi PSYMN,

I have attached the whole model and the errors after hiting the chekc mesh bottom.

Thanks in advance for your help,
Amir
Attached Images
File Type: jpg whole model.jpg (38.3 KB, 31 views)
File Type: jpg Error1.jpg (85.2 KB, 26 views)
File Type: jpg Error2.jpg (92.8 KB, 24 views)
File Type: jpg error3.jpg (39.6 KB, 21 views)
Amir1 is offline   Reply With Quote

Old   August 27, 2013, 18:08
Default
  #10
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 single and multple edge messages are "possible problems" and won't slow down the bottom up tetra meshers.

The non manifold verts might, depending on how the mesh actually looks.

To diagnose better, use the option to create a subset. Then turn off the other mesh displayed and view the subset. Use the subset options to add a layer of shells (do it 2 or 3 times) so you get a better idea of what is going on. If you see any ugly mesh, you can fix it with split edges or merge verts, or even by deleting and recreating a few elements...

Best regards,

Simon
Amir1 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

Old   August 27, 2013, 18:12
Default
  #11
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Hi Simon,

Thanks for your prompt response.
Actually I have tried to use subset but the problem was still there.

Do you have any idea how I can get rid of (thousands) meshes where the strip attaches to the cylinder?

Best,
Amir
Amir1 is offline   Reply With Quote

Old   August 27, 2013, 20:49
Default
  #12
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
If there are thousands of non-manifold verts, I would look at the subset to guess why the were there. Perhaps it is a geometry issue or a mesh size issue (mesh is too coarse). I would fix the issue and remesh.
Amir1 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

Old   August 28, 2013, 15:21
Default
  #13
Member
 
Amir
Join Date: Sep 2012
Posts: 44
Rep Power: 4
Amir1 is on a distinguished road
Hi again,

Do you mind if I send you the geometry file only to take a look at it please?

I created the points then lines. Then surfaces are defined and internal wall were determined.
And then meshing was started.

Thanks
Amir1 is offline   Reply With Quote

Old   August 28, 2013, 22:27
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 Amir,

I took a quick look. The first issue is that you have a tight cusp between the big roller and each moving surface. The top down octree mesher has a hard time with this.

Amir1_01.jpg

You need to set "Thin Cuts". You can find other posts or check the help for more info on thin cuts... A key thing to do is make sure all the curves and points at the intersection between the two parts are in a different part (GEOM).

Amir1_02.jpg


Anyway, it wasn't quite enough, so I also set a smaller size on the curve where the Moving surfaces meet the Roller and also setup a density region in that area... This made it look better, but is still not a good solution.

Amir1_03.jpg

The best solution would be to create some geometry that closes off the tight space. I created some in a part called "INTERFACE". I put a material point inside the cusp region called "FLUID2". Then I setup my prism settings so that FLUID and the INTERFACE were checked, but FLUID2 was not.

Amir1_04.jpg
This was the result (Octree Tetra with Prism)
Amir1_05.jpg
__________________
-----------------------------------------
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   August 28, 2013, 22:28
Default
  #15
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 previous instruction will help with roll1, but the other moving belt passes by two other rollers... Those will need an intersection curve and INTERFACE regions of their own.

In the end, you can put all the FLUID2 elements into the FLUID part and delete the "INTERFACE" shells.

Best regards,

Simon
__________________
-----------------------------------------
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
Fluent msh and cyclic boundary cfdengineering OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 48 January 25, 2013 04:28
Cyclic BC's: Possible face ordering problem? (Channel flow) sega OpenFOAM Native Meshers: blockMesh 3 September 28, 2010 12:46
CheckMeshbs errors ivanyao OpenFOAM Running, Solving & CFD 2 March 11, 2009 03:34
Import gmsh msh to Foam adorean Open Source Meshers: Gmsh, Netgen, CGNS, ... 24 April 27, 2005 08:19
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 19:55.