Inconsistent number of faces between block
Hi,
i'm new to all of these kind of things so forgive if my doubt seems trivial I got these error message while running blockMesh. After some research i found that maybe the problem is in the matching numbers in hex, so i have changed it but the problem wasn't solved. I don't know if there's something missing in the matchPatchPairs() or mergePatchPairs() because i don't understand which cases is it necessary. I'm trying to do a mesh to structure that can be divided in 7 blocks and on top of 3 of them is placed a prism. Can anyone, please help me understand what i'm doing wrong? Code:
convertToMeters 1; |
Hi Chris
A sketch of your geometry would be very helpful. But I think I know the problem and can show a good workaround. I think your mesh contains at least two neighbouring blocks with inconsistent grids... see picture . http://fs2.directupload.net/images/150422/irbf4uky.jpg If you want to avoid mergepatchpairs you have to insert additional blocks... see picture http://fs2.directupload.net/images/150422/uaaope2z.jpg Its the same workaround like in the tutorial cavitatingFoam/throttle . I hope this rather short answer solved your prob. regards Alex |
2 Attachment(s)
Hello Alex, i'm sorry for the delay.
Thank you for your reply, iwas trying to understand what you explained but still i couldn't resolve the problem. Here is the images of what i'm trying to do: to do the blocks hex (0 1 2 3 4 5 6 7) and to the the prism on top of that block hex (7 38 39 6 4 5 4 5) |
1 Attachment(s)
Hi,
I would suggest to divide your mesh like on the attached figure (i.e. using only hexagons). Prismatic blocks are in general PITA (or they just do not like me). |
Ohhh yeah, I see your problem.
Not only that I can confirm alexey's opinion with prismatic blocks... but also you have messed up the grading for your blocks. See User Guide http://cfd.direct/openfoam/user-guid...#x25-1420005.3 Quote:
Quote:
You have to look at every block which direction is your x1,x2,x3 . And then decide the grading in this direction. Perhaps you can blockMesh your grid for a first raw version if you change the grading for all not prismatic blocks from (300 1 60) to (1 60 300) If it works you will see where to change the grading for a better solution and I hope you see the problem with prismatic blocks like predicted by alexey. ;) (in one corner the mesh becomes ultrafine... gives problem with the Courant number in most cases) regards Alex |
The problem isn't only the grading for each block. Also the local coordinates isn't following the right-hand rule. You will get a warning for negative or zero volumes when you fix the grading problem. The mesh will look fine in paraview but the solver will not run.
Bw, Hassan |
Thank you so much for all your help.
Using your suggestions and rewriting blockMeshDict using only hexagons and the right-hand rule, the problem was solved. But then i used checkMesh and got 2 failed mesh checks. So i applied this suggestion: Quote:
Could you please give any tip in how to solve this? |
Hi Chris,
could you attach a sketch of your full grid, and the logs of blockMesh and checkMesh? Perhaps the prob gets clearer for me then. ;) regards Alex |
Attachment 39118Hi Alex,
Here is the logs: Code:
cristina@cristina-HP-Pavilion-g6-Notebook-PC:~/OpenFOAM/cristina-2.2.2/run/test/1$ blockMesh |
This error about the definition of the empty patches. You have many empty patches, the correct one which is frontAndBack only. blockMesh defines the defaultFaces as empty. You have to specify different boundary type for the defaultFaces.
Bw, Hassan |
Thank you. Problem solved.
Using the 13 remaining faces as patch on defaultFaces solved the problem. :) Best Regards Cris Edit: Actually it has to be a wall while running setFields a log message appear saying that it has to be a wall. |
All times are GMT -4. The time now is 04:15. |