CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] Error in mesh writing (http://www.cfd-online.com/Forums/ansys-meshing/114041-error-mesh-writing.html)

helios March 4, 2013 07:31

Error in mesh writing
 
Hi at all, i have a problem with mesh output writing...this is what happens: i choose the solver (fluent v6), then i save my project then the mesh ( uns format) and when i try to configure the fluent menu parameters the following error appears me:

"ERROR

running fluent v6 interface vers 14.5.12

ERROR

the interface cannot handle quadratic elements. child process exited abnormally"

and this is what i see in dialog box:

"WARNING:mesh has uncovered edges. fluent needs a complete boundary( lines in 2d)
or it will give a variety of errors and not read in the mesh. if this was 2D Hexa, perhaps your edges are not associated with perimeter curves".

So how can i see kind of error is?? i guess i have associated all geometry but i have no idea what i have to do to solve the problem. Please help me.

thanks at all

stuart23 March 4, 2013 21:34

http://www.cfd-online.com/Forums/ans...em-fluent.html

*Search first

helios March 5, 2013 07:37

thanks a lot Stuart i'll try and i'll inform you.thanks again

helios March 7, 2013 04:31

4 Attachment(s)
Hi Stuart i've followed advices into post you've been saw me but now i'm still in troui explain you...this is what i've done:

"Turn on all your parts and turn on line elements but turn off shells...
You should have line elements around the perimeter and between any two shell parts...
If not, then that is your problem. The uncovered faces check should also find these.
The fix, if using ICEM CFD Hexa, is to go back and associate edges to curves...
When an edge is associated to a curve, line elements form in the part name of the curve...
No association, no line elements, no boundaries for fluent..." ( FROM SIMON REPLY)

1)i think i have associated all edges to each curve but several errors has been found..
1)all uncovered edges (pict.1)...i'have thought to add that uncovered edges to fluid
(it seems the better solution,doesn't it?)....
2)then the program ask me to choose the surface which contain the periodic faces...
but i don't understand which periodic surfaces it refers(pict2)....
3)icem found many single edge elements located round the airfoil and attached to domain's boundary..
what have i do to fix them?delete them?create a subset and do anything else?(pict3)
4)same question for last problem (pict 4) when icem found standalone elements?
what i have to do to fix them?(pict 4).

I attach pictures and if you can see them i can send you my files...

thanks a lot

Attachment 19646

Attachment 19647

Attachment 19648

Attachment 19649

PSYMN March 8, 2013 11:38

Wow, so much wrong here ;^)

Quadratic elements are elements with mid side nodes. They would be appropriate for FEA analysis in ANSYS or Nastran, but not for CFD codes which require linear elements (no mid side nodes).

ICEM CFD generates linear elements by default, so I am guessing you added mid side nodes at some point... Don't do that.

Your model is not periodic, so no need for the periodic check.

Single edge elements are expected around the perimeter of a 2D model. Just run the check to confirm they are all on the edges (around the far field and around the airfoil) and then be happy. If they are elsewhere, then you have a problem that needs some adjustment.

The other error messages are also not worth worrying about...

If you generated this model with Hexa, just unload your unstructured mesh... Go back to the hexa blocking and confirm that ALL the peirmeter edges are associated with curves. Then convert the premesh to uns mesh again. Smooth again. Run your checks, but don't do anything drastic ;^) Output to the solver...

Best regards,

Simon

helios March 8, 2013 11:48

thanks Simon but if i use quadratic elements without mid side nodes i lose definition around the arfoils...linear elements enter into it and i won't it...how can i do??

PSYMN March 8, 2013 12:35

Fluid solvers only use linear elements (with a few small exceptions). You just have to accept some faceting. The standard solution is a finer mesh in areas of higher curvature so that the facets are smaller and have a smaller max deviation.

helios March 8, 2013 12:46

mmm i see....Simon i appreciate too much your help but i haven't finished to stress you :) i have anothe question: when i use the split edge with autmatic linear option it doesn't work...i have always to use linear option to spread the edge on my curve...why?? and thanks again :)

PSYMN March 8, 2013 13:05

The interactive blocking edge split controls ask you to provide the split vertex. The Automatic Linear option extracts point vertices based on the edge distribution. My guess is that you don't have many nodes along the edge you are trying to split. With no extra nodes for "Automatic Linear" to move, it doesn't appear to do anything. Increase your count on that edge and try again, but be aware that increasing the node count will cause it to propagate out to the model extents.

Best regards,

Simon

helios March 14, 2013 10:54

Hi Simon...have you received my last message??please answer me because i have always the same problem....thanks

Best regards,

Helios

diamondx March 14, 2013 11:23

before using split edge with automatic linear, you need to specify number of nodes on that edge. try it.

helios March 14, 2013 11:37

thanks a lot diamond...i'll try immediately

PSYMN March 14, 2013 11:44

Quote:

Originally Posted by helios (Post 414007)
Hi Simon...have you received my last message??please answer me because i have always the same problem....thanks

Best regards,

Helios

Yes, I replied on the 8th.

helios March 14, 2013 11:48

Sorry Simon i referred to the next message i sent you about an icem's internal error message?? haven't you received it??

mikebausas September 3, 2013 03:51

Hello,

i am working with my thesis where i am trying to simulate the performance of a VAWT with NACA0025 airfoil. I made my mesh in ICEM CFD and successfully imported it to fluent. However, when i am trying to set up my mesh for simulation, the Mesh Interface is grayed out.

Can anyone please help me understand what specifically is the problem and how to fix it. Pls help.. THank you so much in advance.

PSYMN September 3, 2013 08:33

Hey Mike, this looks like a new thread to me. Also, try to be more clear about if you have generated the mesh or not. I thought it was a bit confusing.

karangadani April 6, 2014 06:25

Error in ICEM CFD
 
Error:
Running FLUENT V6 Interface Vers. 15.0.5

Creating a Fluent 2D mesh.
Computing connectivity for 67657 cells.
Error : face (near node 725) is attached to more than 2 cells.
Error : face (near node 739) is attached to more than 2 cells.
Error : face (near node 753) is attached to more than 2 cells.
Error : face (near node 126) is attached to more than 2 cells.
Error : face (near node 101) is attached to more than 2 cells.
Error : face (near node 702) is attached to more than 2 cells.
Error : face (near node 725) is attached to more than 2 cells.
Error : face (near node 753) is attached to more than 2 cells.
Error : face (near node 749) is attached to more than 2 cells.
Error : face (near node 739) is attached to more than 2 cells.
Error : face (near node 730) is attached to more than 2 cells.
Error : face (near node 726) is attached to more than 2 cells.
Error : face (near node 127) is attached to more than 2 cells.
Error : face (near node 690) is attached to more than 2 cells.
Error : face (near node 55) is attached to more than 2 cells.
Error : face (near node 706) is attached to more than 2 cells.
Error : face (near node 706) is attached to more than 2 cells.
Error : face (near node 84) is attached to more than 2 cells.
Error : face (near node 699) is attached to more than 2 cells.
Error : face (near node 698) is attached to more than 2 cells.
Error : face (near node 4810) is attached to more than 2 cells.
Error : face (near node 4810) is attached to more than 2 cells.
Error : face (near node 789) is attached to more than 2 cells.
Error : face (near node 688) is attached to more than 2 cells.
Error : face (near node 699) is attached to more than 2 cells.
Error : face (near node 84) is attached to more than 2 cells.
Error : face (near node 726) is attached to more than 2 cells.
Error : face (near node 654) is attached to more than 2 cells.
Error : face (near node 1274) is attached to more than 2 cells.
Error : face (near node 1274) is attached to more than 2 cells.
Error : face (near node 537) is attached to more than 2 cells.
Error : face (near node 537) is attached to more than 2 cells.
Error : face (near node 4810) is attached to more than 2 cells.
Error : face (near node 101) is attached to more than 2 cells.
Error : face (near node 789) is attached to more than 2 cells.
Error : face (near node 789) is attached to more than 2 cells.
Error in computing cell connectivity.
child process exited abnormally


WARNING: Mesh has uncovered edges. ANSYS Fluent needs a complete boundary (lines in 2D) or it will give a variety of errors and not read in the mesh! If this was 2D Hexa, perhaps your edges are not associated with perimeter curves

can you please help me out how to solve this problem???


All times are GMT -4. The time now is 19:20.