CFD Online Logo CFD Online URL
Home > Forums > ANSYS Meshing & Geometry

unwanted lines after extruding the 2D mesh

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

LinkBack Thread Tools Display Modes
Old   January 5, 2011, 14:05
Default unwanted lines after extruding the 2D mesh
Senior Member
Join Date: Mar 2009
Posts: 102
Rep Power: 9
MASOUD is on a distinguished road
In order to generate a 3D mesh (including 5 zones), I created a 2D surface and then meshed it and extruded this mesh along direction 0 0 1.
Result can be seen in Figure-1.
But looking at the Figure-2 (in which the lowest zone is turned on) and Figure-3 (in which only the CGC-T is visible) there are two unwanted groups of lines with the blue color (the lowest one is wanted and is CGC-T but the other two are unwanted).
I have no idea why these two groups of lines (they are not surface, or surface mesh) are created. Any idea?

The other question: If i import it into Fluent, will they affect the solution procedure/results?

MASOUD is offline   Reply With Quote

Old   January 5, 2011, 14:09
Default Figures
Senior Member
Join Date: Mar 2009
Posts: 102
Rep Power: 9
MASOUD is on a distinguished road
Sorry, I am attaching the figures here.
Attached Images
File Type: jpg 1.jpg (90.2 KB, 18 views)
File Type: jpg 2.jpg (89.0 KB, 14 views)
File Type: jpg 3.jpg (87.1 KB, 10 views)
MASOUD is offline   Reply With Quote

Old   January 8, 2011, 15:39
Default 2D to 3D...
Retired from CFD Online
PSYMN's Avatar
Simon Pereira
Join Date: Mar 2009
Location: Ann Arbor, MI
Posts: 2,660
Blog Entries: 1
Rep Power: 38
PSYMN has a spectacular aura aboutPSYMN has a spectacular aura about
Hey Masoud,

Extrude takes your original mesh and adds a dimension... 2D becomes 3D, 1D becomes 2D, 0D becomes 1D. In other words, shells produce volume elements, lines become side shells, and points become side lines...

So, you must have had that part as line elements in the original 2D mesh, they were simply extruded into 3D shells on the side.

As shells, they certainly will affect your Fluent solution. They could be walls or merely internal walls that separate different volumes (you probably want these). In your case, the same part is used as both an internal and external wall, so you will certainly have a problem. I can really tell, but you may have an even bigger problem if you don't have shells around all the volume elements. Fluent actually needs shells around all volumes (to contain them), and not having them will give a null pointer error.

Go back to your 2D mesh and check that you have line elements around all your shells so that when you extrude, those perimeter lines become enclosing shells around each section. Lines between shells should be in unique parts that can become internal walls in Fluent. The line elements form naturally with the patch conforming mesher, but you must associate edges to curves if you started with Hexa blocking.

For extruding from multiple surfaces, I suggest you use inherited for all the parts (including volume). This will actually put your volume elements in the parts of your shells, but you can then go thru and turn on volume elements and each part and assign the volume elements to a new part manually...

Best regards,

PSYMN is offline   Reply With Quote


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
[ICEM] Negative volume error in hybrid mesh siw ANSYS Meshing & Geometry 4 September 3, 2014 05:25
separating top surfaces after extruding the 2D mesh Mario-CFD ANSYS Meshing & Geometry 3 January 8, 2011 16:26
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
basic of mesh refinement arya CFX 4 June 19, 2007 12:21
Mesh Mignard FLUENT 2 March 22, 2000 06:12

All times are GMT -4. The time now is 16:16.