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

[ICEM] Checking the mesh -> problem of single edges

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 4, 2012, 09:49
Default Checking the mesh -> problem of single edges
  #1
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Hi!

(I apologize for the mistakes)

I'm a beginner regarding ICEM-CFD. I have to mesh a simple 2D axisymetric geometry. My mesh quality is very good (>0.8).
But when I check the mesh, it diagnoses that there are single edge elements. I can delete them, put them in a new subset or ignore. I tried all options but it doesn't work (I can import the mesh in Fluent if I create a new subset, but it doesn't solve my problem) .
When I import my mesh under Fluent, it well appears in the window but when I check the mesh there are errors, and of course I can't run calculation.
If you have any idea to solve this problem, I'd be really grateful!

I have:
- built my geometry
- created different parts my different bocos
- initialized blocking
- splited block to match with my geometry
- associated edges and curves
- associated vertices and points
- updated size (update all)
- pre-meshed
- adjusted edge params
- converted to unstruct mesh
- created bar (element topology) to match with geomtry and parts
- defined my bocos

Thanks a lot,

Clémence
Clecl is offline   Reply With Quote

Old   September 4, 2012, 12:16
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
would you mind sharing your geometry... i can take a look at it
__________________
Regards,
New to ICEM CFD, try this document --> http://goo.gl/G2gkE
Ali
diamondx is offline   Reply With Quote

Old   September 5, 2012, 04:27
Default geometry
  #3
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Thank you for your reply.
I join geometry. Here my mesh is coarse, but it isn't the problem and it changes for single edgesnothing when I refine.
(INLET_TERTIAIRE = there are 2 inlets of tertiary oxygen at the top of the tube
INLET_SECONDAIRE = on the zoom, there is an inlet bottom right
INLET_CHARBON = coal inlet in the middle
INLET_FUMEES = flue gas inlet)

My problem is the presence of single edges when I check the mesh
Maybe I missed a step when I built my mesh?

Thanks a lot again
Attached Images
File Type: jpg general.jpg (25.0 KB, 41 views)
File Type: jpg zoom.jpg (35.8 KB, 35 views)
Clecl is offline   Reply With Quote

Old   September 5, 2012, 04:28
Default
  #4
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
* it changes nothing for single edge when I refine the mesh
Clecl is offline   Reply With Quote

Old   September 5, 2012, 05:23
Default
  #5
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Maybe do a build topology in order to have only red curves.
Then recreate your part with those curves. Maybe you have two curves for the same part.
You should not have a GEOM part by the way.

Single edge is a possible problem. I don't know how FLUENT works, but maybe the problem doesn't come from the single edges.
BrolY is offline   Reply With Quote

Old   September 5, 2012, 07:26
Default
  #6
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Thank you, I'm going to try this, I'll tell you later if it is the solution!
Clecl is offline   Reply With Quote

Old   September 5, 2012, 09:00
Default
  #7
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Do you mean that I have to a build diagnostic topology (in "Repair Geometry")? (I tried this, but I don't know which option I had to choose)
Clecl is offline   Reply With Quote

Old   September 5, 2012, 10:05
Default
  #8
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Yes : Geometry -> Repair Geometry -> Build Diagnostic Topology

Tolerance should be something as 10 time your smallest element mesh size.
Select the option "join edge curves".
BrolY is offline   Reply With Quote

Old   September 5, 2012, 11:46
Default
  #9
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
The geometry look very simple. Can you upload the tin file?
yonchong is offline   Reply With Quote

Old   September 6, 2012, 03:24
Default
  #10
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Yes it is! But even with an easier geometry I have the problem of the single edges (I tried with a square yesterday...). I don't understand where I'm wrong...
I join the tin file.
I tried the build diagnostic geometry as you told me Alexandre, but it deleted my inlet of tertiary oxygen (even if I put a very small tolerance). I'll try again, maybe I have done a mistake.
Thanks again!
Attached Files
File Type: zip essai2000.tin.zip (1.4 KB, 3 views)
Clecl is offline   Reply With Quote

Old   September 6, 2012, 08:11
Default
  #11
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
I am sorry. I forgot to ask the blk file as well.
yonchong is offline   Reply With Quote

Old   September 6, 2012, 08:30
Default
  #12
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Here it is!
I fail and fail, and I don't understand why ... Don't hesitate if you have any idea to get me out of there!!
Thank you (again )
Attached Files
File Type: zip essai4000.blk3.zip (2.4 KB, 1 views)
Clecl is offline   Reply With Quote

Old   September 6, 2012, 08:34
Default
  #13
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
I forgot the corresponding geometry
Attached Files
File Type: zip essai4000.tin.zip (1.5 KB, 2 views)
Clecl is offline   Reply With Quote

Old   September 6, 2012, 08:50
Default
  #14
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
Actually, I found what your problem is.

It is a 2-D mesh you are trying to generate and you don't have surfaces. You use bodies for 3-D mesh.

I don't know how you created the geometry but you can go back and output that or if it was generated in ICEM then follow the step to generate a surface.
  1. Geometry -> Create/Modify Surface -> Simple Surface (give a part name and select all curves and Apply)
  2. Geometry -> Create/Modify Curve -> Project Curve on surface (give a part name and select all curves and the newly created surface)
  3. Geometry -> Create/Modify Surface -> Segment/Trim Surfaces (give a part name and select all curves and the newly created surface)
  4. You may choose to move the newly created geomety to the old part and delete the old geometry. Also delete unwanted surfaces.
  5. I am not sure whether you can read in the blocking file and reuse it but if not you might have reassociate all the curves and points.
  6. Remesh.
You will get single edges at the boundary because the line element will have only one shell element. However this is ok. Just output the mesh to Fluent and check the mesh.
yonchong is offline   Reply With Quote

Old   September 6, 2012, 08:57
Default
  #15
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
In fact, you might try

Repair Geometry -> Build Diagnostic Topology

after creating the surface. I might automatically project the curves to the surface and segment the surface for you.
yonchong is offline   Reply With Quote

Old   September 6, 2012, 09:57
Default
  #16
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Thank you. I tried this with my current geometry but it failed (when I check the mesh in fluent, "check mesh failed").
But I am starting a new project (I restart from the beginning to avoid mistakes) where I am going to follow your procedure, I hope it will work!
I'll tell you if it was the solution.
Thank you very much anyway!
Clecl is offline   Reply With Quote

Old   September 6, 2012, 10:00
Default
  #17
Member
 
Yon Han Chong
Join Date: Jun 2012
Posts: 77
Rep Power: 5
yonchong is on a distinguished road
Did you deleted the old geometry?

I have built a mesh as I have described using unstructed mesher and read into Fluent without any error.

Good luck with your new project though.
yonchong is offline   Reply With Quote

Old   September 6, 2012, 10:59
Default
  #18
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
There is no error when I check the mesh if I choose 2D planar in general model in Fluent. If I choose Axisymetric or Axisymetric Swirl, check mesh failed!

Thank you for your help, maybe I can run my simulations with 2D planar, we'll see!
Clecl is offline   Reply With Quote

Old   September 21, 2012, 05:48
Default
  #19
Senior Member
 
AB
Join Date: Sep 2009
Location: France
Posts: 323
Rep Power: 12
BrolY will become famous soon enough
Sorry, I was in holiday and wasn't able to answer to you before.

1) You don't have any surface, so that won't work. Even if it's a 2D scenario, you need surface (as you need volume when it's a 3D scenario).
2) If I understand your project, there are 2 inlets which are ponctual (mean modelled by a point), 2 inlets which are linear (mean modelled by a curve).
I guess this is more a solver issue than a mesher issue. How do you model ponctual source with your solver ? Maybe it's by coordinate ? Are you sure you need to specify a point within your mesher ?
3) The geometry is very simple, so your blocking is OK.
4) Try to run your simulation without any symmetry first, and see if it's work.
Next, you will have to define which part is symmetry etc ... But, you should first try to acheive a simple simulation.
BrolY is offline   Reply With Quote

Old   September 21, 2012, 08:38
Default
  #20
New Member
 
Join Date: Sep 2012
Posts: 13
Rep Power: 4
Clecl is on a distinguished road
Thank you for your reply.
I finally found my mistake a week ago: my axis was not the X-axis, so it didn't work on Fluent with the Axissymmetric model (because the axis of symetry have to be the X-axis on Fluent, I don't know why).
I have always single edges, but I think it's not a problem for Fluent, because the check mesh on Fluent is OK.
All my inlets are curves, but some are very very small.
Now I have other problems on Fluent, so I have to ask to an other forum !
And thank you to Yonchong, you allowed me to continue my project!
Clecl 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
CGNS converters available mbeaudoin OpenFOAM Meshing & Mesh Conversion 125 July 1, 2015 21:09
[ICEM] Problem making structured mesh on a surface froztbear ANSYS Meshing & Geometry 4 November 10, 2011 09:52
[ICEM] Problem making structural mesh on a surface froztbear ANSYS Meshing & Geometry 1 November 10, 2011 09:52
Problems in compiling paraview in Suse 10.3 platform chiven OpenFOAM Installation 3 December 1, 2009 08:21
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 02:14.