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] Problems with meshing a 3D wing w/winglet (http://www.cfd-online.com/Forums/ansys-meshing/114780-problems-meshing-3d-wing-w-winglet.html)

cesarcg March 17, 2013 17:13

Problems with meshing a 3D wing w/winglet
 
Hi all,

I'm having problems meshing a 3D wing with a winglet using hexa-mesh. I finished the blocking and ran a quality check for premesh based in determinant and angle criteria and obtained above 0.4 and 19║, respectively. Then I proceeded to convert the premesh to an unstructured mesh.

After the mesh was generated, I ran a quality check for all the cells based in determinant, min angle, and orthogonal quality and obtained above 0.4, 19║, and 0.35, respectively. The problem here is that Icem is printing a message about 5028 cells with undefined quality during each check. I also did a check for problems finding out that there are 10 penetrating cells that can be fixed without improving the issue about the undefined quality cells. Geometry and blocking files are below:

https://www.dropbox.com/s/hw85r1x1n8...luidDomain.tin
https://www.dropbox.com/s/uffxplfl5x...013_Coarse.blk

Does anybody know how to locate these undefined quality cells in order to fix them? I need to solve this since the mesh is giving me problems in Fluent because they are detected as cells of low orthogonal quality (below 0.01) and I blame these ones to the instability and difficulty to convergence of numerical solution. I hope someone can help me out with this since it is part of my dissertation and I'm running out of time.

Thanks in advance,
CÚsar

Pospelov March 17, 2013 17:54

Hello, Cesarcg!
You blocks is very good!
You should try check your grid by determinate 3x3x3 in rang -1 to 1. I think you will see your error there.
Pospelov Alexander

cesarcg March 17, 2013 18:20

Quote:

Originally Posted by Pospelov (Post 414544)
Hello, Cesarcg!
You blocks is very good!
You should try check your grid by determinate 3x3x3 in rang -1 to 1. I think you will see your error there.
Pospelov Alexander

Hi Alexander,

Thanks for your suggestion but I already did that and didn't find the error. I ran out of ideas to look for the problem.

Regards,
CÚsar

Pospelov March 17, 2013 19:32

If you delete part solid, you would not have any problem in ICEM. I've done all checks in ANSYS 13.0.
But it's takes me some time, because I've got not good computer at home. )
Pospelov Alexander

Far March 18, 2013 03:12

Excellent. Outclass.

diamondx March 18, 2013 10:55

Still i think tetra+prism is more suitable for this. multizone will be the best. a premesh info inform me that you have generated 9 000 000 nodes. you really need some strong hardware there to simulate this...

Far March 18, 2013 11:00

@Ali. No of nodes can be reduced as I can see many refinements in unimportant areas. And I like the blocking strategy...

diamondx March 18, 2013 11:04

the blocking is perfect of course

kad March 18, 2013 11:25

One possible solution could be to deactivate line_2 elements while running quality checks. Quality is of course not defined for line elements.

cesarcg March 18, 2013 12:42

Quote:

Originally Posted by Pospelov (Post 414565)
If you delete part solid, you would not have any problem in ICEM. I've done all checks in ANSYS 13.0.
But it's takes me some time, because I've got not good computer at home. )
Pospelov Alexander

Hi Alexander,
Thanks for your suggestions. I followed what you've recommended but I just figured out that my problem may not be because the part solid present during unstructured mesh generation neither the translator to mesh for fluent. I ran the mesh quality check before and after export the mesh to fluent and ICEM and got the same minimum values for the different criteria (min angle=21.4║, min determinant=0.35, and min orthogonal quality=0.24). So I guess there is no problem with ICEM.
I think this values are good enough to run the simulation with no big problems, but when read the mesh in fluent, it prints that the orthogonal quality mesh is low (7.35845e-3). I think that I should make a check with gambit and see what it tells.

Quote:

@Ali. No of nodes can be reduced as I can see many refinements in unimportant areas. And I like the blocking strategy...
Hi Far,
Hope that you are doing great. Can you tell me where the number of nodes can be reduced according to your experience? I know that there are some regions that can be improved and your advices would be very helpful.

Quote:

One possible solution could be to deactivate line_2 elements while running quality checks. Quality is of course not defined for line elements.
Hi Kad,
I did what you suggested and you are right. I didn't know that. Thanks a lot.

---------------------
Thanks to everyone,
CÚsar

Far March 18, 2013 13:12

Quote:

Thanks for your suggestions. I followed what you've recommended but I just figured out that my problem may not be because the part solid present during unstructured mesh generation neither the translator to mesh for fluent. I ran the mesh quality check before and after export the mesh to fluent and ICEM and got the same minimum values for the different criteria (min angle=21.4║, min determinant=0.35, and min orthogonal quality=0.24). So I guess there is no problem with ICEM.
I think this values are good enough to run the simulation with no big problems, but when read the mesh in fluent, it prints that the orthogonal quality mesh is low (7.35845e-3). I think that I should make a check with gambit and see what it tells.
Check other parameters like volume change, dihedral angle. And identify areas in Fluent by looking at contour plot of orthogonal quality and improve that area in ICEM.



Quote:

Hi Far,
Hope that you are doing great. Can you tell me where the number of nodes can be reduced according to your experience? I know that there are some regions that can be improved and your advices would be very helpful.
Spanwise mesh is not important as compared to normal to surface mesh is. Inlet and outlet areas in far-field are less important, reduce mesh there.


All times are GMT -4. The time now is 13:19.