CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (https://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Checking the mesh -> problem of single edges (https://www.cfd-online.com/Forums/ansys-meshing/106640-checking-mesh-problem-single-edges.html)

 Clecl September 4, 2012 09:49

Checking the mesh -> problem of single edges

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
- converted to unstruct mesh
- created bar (element topology) to match with geomtry and parts
- defined my bocos

Thanks a lot,

Clémence

 diamondx September 4, 2012 12:16

would you mind sharing your geometry... i can take a look at it

 Clecl September 5, 2012 04:27

geometry

2 Attachment(s)
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

 Clecl September 5, 2012 04:28

* it changes nothing for single edge when I refine the mesh

 BrolY September 5, 2012 05:23

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.

 Clecl September 5, 2012 07:26

Thank you, I'm going to try this, I'll tell you later if it is the solution!

 Clecl September 5, 2012 09:00

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)

 BrolY September 5, 2012 10:05

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".

 yonchong September 5, 2012 11:46

The geometry look very simple. Can you upload the tin file?

 Clecl September 6, 2012 03:24

1 Attachment(s)
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!

 yonchong September 6, 2012 08:11

I am sorry. I forgot to ask the blk file as well.

 Clecl September 6, 2012 08:30

1 Attachment(s)
Here it is!
I fail and fail, and I don't understand why :confused:... Don't hesitate if you have any idea to get me out of there!!
Thank you (again :))

 Clecl September 6, 2012 08:34

1 Attachment(s)
I forgot the corresponding geometry

 yonchong September 6, 2012 08:50

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 September 6, 2012 08:57

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.

 Clecl September 6, 2012 09:57

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!

 yonchong September 6, 2012 10:00

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.

 Clecl September 6, 2012 10:59

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!

 BrolY September 21, 2012 05:48

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.

 Clecl September 21, 2012 08:38