[asal]

Hello everybody

I want to know how can I save all the boundary conditions and setting in FLUENT 14.0 in order to use them in other mesh.
I have several meshes for the same geometry. When I assign all the bounday conditions, then I want to save these setting and load for the others to avoid setting again for all of the meshes.
thanks.

[mrenergy]

Hi asal,

save your boundary conditions and other setting in FLUENT in a case file,

the case file will be saved including the mesh that it saved on.

so ...

file > read > case

then file > read > mesh > replace mesh

the mesh will be replaced while all other bc and run settings will be kept.

I tried it now to be sure, as I am a new FLUENT user, it works.

GOOD LUCK

Mamdouh

[asal]

Hello and thanks for your reply.

I found another solution which could be interesting:

To save all currently defined boundary conditions to a file, enter the file/write-bc text command and specify a name for the file.

file write-bc

ANSYS FLUENT writes the boundary and cell zone conditions, the solver, and model settings to a file using the same format as the "zone'' section of the case file. See Appendix B for details about the case file format.

To read boundary conditions from a file and to apply them to the corresponding zones in your model, enter the file/read-settings text command.

file read-settings

ANSYS FLUENT sets the boundary and cell zone conditions in the current model by comparing the zone name associated with each set of conditions in the file with the zone names in the model. If the model does not contain a matching zone name for a set of boundary conditions, those conditions are ignored.

If you read boundary conditions into a model that contains a different mesh topology (e.g., a cell zone has been removed), check the conditions at boundaries within and adjacent to the region of the topological change. This is important for wall zones.



Note: If the boundary conditions are not checked and some remain uninitialized, the case will not run successfully.

When the file/read-settings text command is not used, all boundary conditions get the default settings when a mesh file is imported, allowing the case to run with the default values.

If you want ANSYS FLUENT to apply a set of conditions to multiple zones with similar names, or to a single zone with a name you are not sure of in advance, you can edit the boundary-condition file saved with the file/write-bc command to include wildcards ( *) within the zone names. For example, if you want to apply a particular set of conditions to wall-12, wall-15, and wall-17 in your current model, edit the boundary-condition file so that the zone name associated with the desired conditions is wall-*.

[mrenergy]

Nice,

Beside, to advance both procedures, a FLUENT journal file may be built to repeat these steps for many cases ...

read mesh ... apply saved b-c settings (or read case file) ... run ... save ... read another mesh ... and so on

but I am still seeing my suggestion is more easier and efficient

GOOD LUCK

Mamdouh

[ujwal rajan]

Hey guys!

I am relatively new in fluent and i am trying to read and apply velocity and angle profiles into fluent using text user interface.
I have managed to read the velocity profile but i am unaware about how to apply the already read profile onto a specific zone.
Can anyone provide me with the command and syntax to apply the profile??

Thank you!
Help is massively appreciated!