CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Export boundary setting in Fluent 14.0

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes
  • 2 Post By mrenergy
  • 2 Post By asal

Reply
 
LinkBack Thread Tools Display Modes
Old   February 5, 2013, 01:23
Default Export boundary setting in Fluent 14.0
  #1
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 149
Rep Power: 4
asal is on a distinguished road
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.
asal is offline   Reply With Quote

Old   February 5, 2013, 08:03
Default
  #2
Member
 
Mamdouh
Join Date: Dec 2012
Location: Calgary, Alberta, Canada
Posts: 39
Rep Power: 3
mrenergy is on a distinguished road
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
virgy and asal like this.
mrenergy is offline   Reply With Quote

Old   February 10, 2013, 07:35
Default Reading and Writing Boundary Conditions
  #3
Senior Member
 
Astio Lamar
Join Date: May 2012
Location: Pipe
Posts: 149
Rep Power: 4
asal is on a distinguished road
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 and AdamAL like this.
asal is offline   Reply With Quote

Old   February 10, 2013, 08:07
Default
  #4
Member
 
Mamdouh
Join Date: Dec 2012
Location: Calgary, Alberta, Canada
Posts: 39
Rep Power: 3
mrenergy is on a distinguished road
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
mrenergy is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Water subcooled boiling Attesz CFX 7 January 5, 2013 03:32
Residual level setting of Fluent lhlh ANSYS 2 November 17, 2012 21:35
Setting outlet Pressure boundary condition using CAFFA code Mukund Pondkule Main CFD Forum 0 March 16, 2011 04:23
asking for Boundary condition in FLUENT Destry FLUENT 0 July 27, 2010 00:55
Help setting up Fluent for a rotor blade Fluent learner FLUENT 3 July 11, 2006 12:01


All times are GMT -4. The time now is 06:43.