Mesh files are created using the mesh generators (Ansys Meshing, the meshing mode of Fluent, Fluent Meshing, GAMBIT, GeoMesh, and PreBFC), or by several third-party CAD packages. From the point of view of Ansys Fluent, a mesh file is a subset of a case file (described in Reading and Writing Case Files). The mesh file contains the coordinates of all the nodes, connectivity information that tells how the nodes are connected to one another to form faces and cells, and the zone types and numbers of all the faces (for example, wall-1, pressure-inlet-5, symmetry-2).
The mesh file does not contain any information on boundary conditions, flow parameters. For information about meshes, see Reading and Manipulating Meshes.
To read a native-format mesh file (that is, a mesh file that is saved in the Ansys Fluent format, which includes FLUENT 5/6, Fluent/UNS, or RAMPANT meshes) into Fluent, use the File/Read/Mesh... ribbon tab item.
File → Read → Mesh...
Note that you can also use the File/Read/Case... ribbon tab item (described in Reading and Writing Case Files), because a mesh file is a subset of a case file. Ansys Meshing, the meshing mode of Fluent, Fluent Meshing, GAMBIT, and GeoMesh can all write a native-format mesh file. For information about these files and how they are created, see Ansys Meshing Mesh Files, Fluent Meshing Mode Mesh Files, Fluent Meshing Mesh Files, GAMBIT Mesh Files, and GeoMesh Mesh Files.
If after reading in a mesh file (or a case and data file), you would like to read in another mesh file, the Read Mesh Options Dialog Box will open, where you can choose to
Discard the case and read in a new mesh.
Replace the existing mesh.
You also have the option to have the Scale Mesh dialog box appear automatically for you to check or scale your mesh, which in general is the recommended practice. For this to happen, enable Show Scale Mesh Panel After Replacing Mesh.
By default, when reading mesh files, Fluent uses the Common Fluids Format (CFF) which is built on the Hierarchical Data Format (HDF5). To read CFF files, use the ribbon tab item or text command and simply append .msh.h5 to the file name.
Note: In order to avoid changing preferences when reading mesh files, while using the Select File dialog box, as long as the file exists, Fluent will respect your choice of file regardless of the type that is selected for the Files of type field. Even if there is no explicit file type extension provided when specifying a mesh file, Fluent will initially look for a .msh.h5 file type, followed by a .msh.gz file type, and finally a .msh file type.
CFF and HDF files are always binary and make use of built-in compression. Thus, they cannot be viewed in a text editor. However, third-party tools are available that enable you to open and explore the contents of files saved in HDF format.
You can read legacy mesh files (with the .msh extension) using one of the following options:
When reading mesh files using the File/Read/Mesh... ribbon tab item, you can look for files written in the legacy mesh format by selecting All Mesh Files (*.msh* *.MSH*) from the Files of type drop-down list in the Select File dialog box.
To read legacy mesh files in the current session, you can use the following text command:
file/cff-files? no; to read legacy mesh files in the current and future sessions, open the General tab of the Preferences dialog box and select Legacy from the Default Format for I/O drop-down list. Note that both of these actions will also result in you reading and writing legacy case and data files.
For information on importing an unpartitioned mesh file into the parallel version of Fluent using the partition filter, see Using the Partition Filter.
For information about reading surface mesh files, see Reading Surface Mesh Files.