CFD Online Discussion Forums

CFD Online Discussion Forums (
-   ANSYS Meshing & Geometry (
-   -   [ICEM] how can i delect the duplicate mesh line and nodes in interface between quad and tri? (

snailstb November 21, 2009 09:13

how can i delect the duplicate mesh line and nodes in interface between quad and tri?
I create two domains, quad is created in the inner domain in order to get good quality of meshes, tri is the other one to smooth and remesh( because tri is good for large distortion for moving body).

i did it according to
here is the steps:
1. create qurd meshes, open the dot nodes, the line nodes are green,like w1.
2. create tri meshes, like w2.
3. merge two domain meshes
4. load to fluent,warning appeared, the interface between tri and quad domians named sbox separate into two, and unfortunately, these two interfaces became wall in boundary condition panel。

"Note: Separating wall zone 12 into zones 12 and 1.
sbox -> sbox (12) and sbox:001 (1)"

i set sbox as interior (i mean the mesh nodes and lines are shared by two domains) in ICEMCFD, but when it is loaded into fluent,
error appears:

"Warning: Inappropriate zone type (interior) for one-sided face zone 1.
Changing to wall.
Warning: Inappropriate zone type (interior) for one-sided face zone 13.
Changing to wall.

Error: Cannot change int_sbox:001 to interior because
there is only one adjacent cell thread."

how can i do to accomplish that only one interior cells between two domains? It can be easily got in gambit.

thanks a lot, it torments me for a long time.

snailstb November 21, 2009 10:00

3 Attachment(s)
the corrseponding pictures are showed as follow:

snailstb November 21, 2009 11:08

5 Attachment(s)
actually, after the quad meshes creating, it needs to export. because,when tri meshes are creating, quad cells will be touched and disappear in ICEMCFD, no matter whether the " respect line elements" select or not, i do not why?

gambit can easily get the conforming meshes in the interface whose mesh nodes and lines are shared between quad cells domain and tri cells domain. what can i do in ICEMCFD?


snailstb November 21, 2009 22:22

can anybody help me? this problem bother me for a long time. thank you all

PSYMN November 23, 2009 16:21

I don't know what went wrong off the top of my head, but if you want to send me the ICEM CFD files (privately), I can take a look and correct your process.


snailstb November 27, 2009 12:54


Originally Posted by PSYMN (Post 237394)
I don't know what went wrong off the top of my head, but if you want to send me the ICEM CFD files (privately), I can take a look and correct your process.


i am very pleased for your reply, i found a way to solve this problem, that is selecting the int wall in part mesh setup, and then go to fluent set up toolbar to define it the interior zone. when loaded in fluent, the interface wall change into the interior wall.
above is the 2d method to deal with the confromal nodes mesh.

when 3d meshing, merge nodes method is used, the meshes will translate through pyramid meshes between hex and tet

thank you all the same. simon, sincerely hope you can help me , because i confronted many problems i do not know how to solve in ICEMCFD.

PSYMN November 28, 2009 00:03

Glad you were able to sort it out.
Well then, until the next time, good luck ;)

DarrenC February 23, 2010 01:16

Hi snailstb,

Im kind of in the same boat as you except my problem is in 3D. I am using ICEM 12 to merge both my tet and hex mesh together using merge nodes>merge meshes. I just select the surface that has been meshed on by the two types of meshes and running a cut plane through shows that the elements have merged (i.e pyramids at the interface).

I then export this mesh to Fluent and Fluent splits this surface into 2 walls (name-shadow, name). Normally when this happens in 2D, i just had to change it to interior and one of the duplicates disappear. But now in 3D when I convert it to a wall, i get the following message "Cannot change name-shadow to interior because adjacent cell threads are of different types." Have u ever get this error message before?

Thanks for your help


DarrenC February 23, 2010 01:58

Found the problem. I just realised in my cell zone conditions that one of my zone was solid and the other one was fluid. Just change both to fluid and the problem is fixed.

mikebausas September 26, 2013 03:10

Simon, I am working on a three bladed VAWT for my thesis. I already built 1/3 of my turbine and subsequently generated its pre-mesh which i then converted to unstructured mesh. My problem now is, when i try to copy rotate the mesh and merge the nodes, only the original 1/3 portion has the line elements. It would not appear to the other two copy rotated parts. I am trying to fix the problem by checking the mesh and fixing uncovered faces. However, the airfoil boundaries would also join the line elements for the inner fluid interface. Please help me so that i can go forward with my work.. Thanks so much in advance.

PSYMN September 26, 2013 08:19

I assume it is your original sector that has the line elements.

My first guess would be that you simply did not select them when you tried to apply the copy rotate. Perhaps the parts were not on and you box selected or selected visible? Next time try the option to "select all".

All times are GMT -4. The time now is 16:58.