[nkalkote]

Hello guys,

Does anyone know a link or reference to a document which explains how elements and their connectivity is stored in openfoam mesh file.

Currently our solver supports .cgns files. we are looking forward to read and write openfoam meshes.

Thanks!!

[windscion]

OpenFOAM is designed to obscure the fact that this starts out fairly simple. Also, the documentation is very much piecemeal, but chapter 5 of the user guide is a good place to start.

Run a tutorial (any tutorial) then look under constant/polyMesh. There will be at least five files:

• boundary
• points
• faces
• owner
• neighbour

As long as these are in ASCII format, they are mostly self-explanatory.

'points' simply lists vertices in 3d.
'faces' lists faces generated by tracing a given set of vertices in order.
'owner' and 'neighbour' list the owner and non-owner cells which are connected by the given face. Faces without neighbour cells are exterior faces, and must be part of a boundary (see the 'boundary' file). You can denote a lack of neighbour either with a -1 or by simply truncating the neighbour file. This is why the neighbour file is often much shorter than the owner file. Also, for a given face the index of owner must be less than the index of neighbour. Plus, the face vector must point out of the owner cell.

For boundary, know that the order of the faces must be:

interior faces (no entry in boundary file)
first patch
second patch
...
last patch

*****************

Also, see
https://www.cfd-online.com/Forums/op...mpactlist.html

for faceCompactList and how to adjust for it.

******************

Some meshes included Zones and crap that I never use, good luck with those.

[elvis]

Hi,
just my 2 cent
take a look at
https://openfoamwiki.net/index.php/S...GNS_Converters

there i a commercial tool as well
https://www.cfd-online.com/Forums/op...converter.html