[evan247]

Dear all,

I was trying to use Fine Turbo to run a multistage turbine passage and experienced below error message at the start of my run:

TYPE OF BC WITH SIX INDECES : 2 13 13 1 41 1 53
CONNECTED DOMAINS WITH SIX INDECES : 5 13 13 -1 -1 -1 -1
!createBcBranch : ERROR IN THE FOLLOWING CONNECTED BC INDICES
! 15 -1 -1 15 -1 -1
! 13 13 -1 -1 -1 -1

My mesh was generated in IGG and I've checked all the connected patches and don't think there should be any problems with them. Could anyone point out what these indices refer to?

Thanks much,
evan

[DarylMusashi]

You may try to check your .std file in your calculation directory. Just open it with the windows standard editor. Maybe there is a more detailed error description. You can post it here, if there are more information concerning your problem.

I don't know how much time and effort you already spent in your mesh generated with IGG. An option could be to use AutoGrid 5 instead, you will get a high quality mesh in relatively short time. In general it is no problem to get a 4 weeks test-license from your NUMECA vendor of your region/country. That should be enough time to generate your mesh.

But I am afraid it is difficult to help you without having a look at your mesh. Another option would be to contact your local NUMECA support team to help you. Even if you do an academical project a limited support should be granted.

[Hamidzoka]

Dear Evan;
Fine turbo sometimes has problems with FNMBs (full non-matching boundary).
FNMBs are interfaces in which sides have different mesh distributions. Try removing FNMBs through changing the mesh settings in Autogrid. if not successful, leave the mesh distribution process to Autogrid by only setting the desired number of elements per set. This generally solves the problem.
does it help?

regards

[evan247]

Originally Posted by Hamidzoka

Dear Evan;
Fine turbo sometimes has problems with FNMBs (full non-matching boundary).
FNMBs are interfaces in which sides have different mesh distributions. Try removing FNMBs through changing the mesh settings in Autogrid. if not successful, leave the mesh distribution process to Autogrid by only setting the desired number of elements per set. This generally solves the problem.
does it help?

regards

Thanks for your reply - I checked all my boundary conditions in IGG and there were no NMB patches. I also tried to simulate only one stage but all gave me the same error as stated in my OP. In the .std file I got below messages (in the end of the file):

createControlSurfaceList: number of entries = 2
createControlSurfaceList: surf INLET id 1
createControlSurfaceList: surf EXIT id 0
cbcinc: create 0 spaces in NMBSubPatchList

I wonder what the last line means.

Also a side question is: is there an easy way to just save the mesh for one / a group of blocks? Or do I have to delete all other blocks and save them one by one?

Thanks in advance.

Evan

[colinda1]

The indices refer to the patches that are causing the problem:
2 13 13 1 41 1 53 is the patch of block 2 that is connected to a patch of block 5. Negative indices for the patch seem strange to me though. If there should be only matching connections in your mesh you could set all CON connections to undefined and search them using the button "Search" in the boundary conditions menu to see whether it correctly finds all of them. If you still have UND patches after the search, you need to take a closer look at these. Normally it should not be necessary to define connections manually.

Best regards,
Colinda

[evan247]

Originally Posted by colinda1

The indices refer to the patches that are causing the problem:
2 13 13 1 41 1 53 is the patch of block 2 that is connected to a patch of block 5. Negative indices for the patch seem strange to me though.

Hi Colinda,

Thanks very much for your reply. I checked block 2 and 5 again and the connecting patches seemed fine. In my OP the error message was:

!createBcBranch : ERROR IN THE FOLLOWING CONNECTED BC INDICES
! 15 -1 -1 15 -1 -1
! 13 13 -1 -1 -1 -1

I wonder if they refer to block 13 and 15? I did check those too but in vain.

[Hamidzoka]

Hi Evan;
As far as I know, you should delete the blocks and keep only the required ones for the means of saving.
Does your airfoils have complicated features like cutbacks, blade tip complicated geometries or endwall fillets?
if yes, remove them and remesh the geometries.
keep the airfoil geometries as simple as possible, but still accurate. "Autoblade" (one of NUMECA modules), if available, can be helpful for this purpose. Sometimes imported geometries from CAD models brings about some small discontinuities that can interrupt the structured automated meshing process in "Autogrid".
if it does not work, as a test only, try removing the tip clearances of rotating blades.
does it help?

Regards

[einandr]

Hi everyone!
I got the same error, problem indicated in log file - it is multigrid related. Strangely, when I create project through GUI it seems internally corrected multigrid settings. When I create project thorugh script in batch, it gives error when trying to run batch solution. First I used 2 3 2 directions multigrid for 2 general level. Then I corrected to 1 1 1 directions with 1 general multigrid level and it run without problem.

!ERROR IN COARSENING OF CONNECTED BLOCKS 7 AND 13
!ON GRID LEVEL 1
!NUMBER OF POINTS FOR THE FOLLOWING INDICES
!DO NOT MATCH
! 1 1 5 5 6 5
! 3 1 14 1 6 14
! Please check if the mesh allows more than 1 multigrid level(s) on each block