Directed meshes from Star-CCM+ not working properly

Questions and remarks about code_saturne usage
Forum rules
Please read the forum usage recommendations before posting.
Post Reply
saintlyknighted
Posts: 13
Joined: Sun Aug 06, 2023 3:40 am

Directed meshes from Star-CCM+ not working properly

Post by saintlyknighted »

Hi all,

I am currently trying to use Star-CCM+ to generate some coarse meshes to use in Code_Saturne. Usually in Star-CCM+ you would use the Automated Mesh option with different parameters to automatically generate the mesh that you want, but I need to use the Directed Mesh option as I need to (semi) manually generated a customised mesh pattern for my geometry.

I have successfully run simulations using automated meshes from Star-CCM+ imported into Code_Saturne before, using the CGNS format. However, as for directed meshes, I can successfully import the meshes to be read in Code_Saturne, but the boundary conditions that I specify (in the GUI) don't seem to be working - I specified an inlet velocity but the entire fluid domain remains static. I've followed the same procedure for both an automated and directed mesh for the same geometry but that the simulation works with the automated one and not the directed one. Not entirely sure what's going so I figured I'd just ask here, if there's anyone that's familiar with Star-CCM+ meshing that might be helpful too.

I've attached the two mesh files of a simple cubic fluid domain, one automated and one directed, as well as the .xml file of the Code_Saturne simulation.
Attachments
setup.xml
(7.3 KiB) Downloaded 185 times
block_directed.cgns
(118.19 KiB) Downloaded 195 times
block_automated.cgns
(186.06 KiB) Downloaded 199 times
Yvan Fournier
Posts: 4102
Joined: Mon Feb 20, 2012 3:25 pm

Re: Directed meshes from Star-CCM+ not working properly

Post by Yvan Fournier »

Hello,

Looking at the directed file with a generic CGNS utility (cgnsview), it appears the boundary zone info is not present in the CGNS file, so your boundary conditions specify nonexistent zones, and BCs default to wall. Which explains why nothing happens in the simulation.

So this is definitely either a Star-CCM+ user issue (specific options missing ?), or a bug if no options are supposed to be required.

Note that in older versions of CGNS (not sure if this si still the case), you could only define node-based BCs and not face-based BCs for structured meshes in the CGNS standard. So if Star-CCM+ lets you choose between face and node/vertex-based BCs, you can try exporting them as node-based BCs. Using the CGNS format (and only for thart format), code_saturne will convert back to face-based BC's automatically (if some BC zone info is present in the file).

Note also that if you have multiple blocks, code_saturne will not manage the block to block mapping in of (only issuing a warning), so you will need to use the mesh joining options to rebuild that info in code_saturne.

Best regards,

Yvan
saintlyknighted
Posts: 13
Joined: Sun Aug 06, 2023 3:40 am

Re: Directed meshes from Star-CCM+ not working properly

Post by saintlyknighted »

I seem to have resolved the issue, turns out I had to specify the region boundaries in the export mesh window in Star-CCM+. Odd because it didn't require me to do that with automated meshes. But yes, thanks Yvan for pointing me in the right direction, the cgnsview utility was pretty helpful in observing whether the mesh going to work or not.
Post Reply