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

Pre in batch mode

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 13, 2007, 01:12
Default Pre in batch mode
  #1
Kuts
Guest
 
Posts: n/a
Hello All,

Can any one suggest me how to do the following. I have many number of mesh files for one geometry, in which one geometrical parameter varies for each case. I have a session file to set the boundary conditions. How can I read the mesh file, use the session file to apply boundary condition and then write the def file in batch mode. I don't want to open the CFX Pre GUI at all. Is there any single command to do this?

Hope to hear from you, Kuts
  Reply With Quote

Old   August 13, 2007, 01:42
Default Re: Pre in batch mode
  #2
hdj
Guest
 
Posts: n/a
Hello Kuts,

To generate def file try this:

cfx5gtmconv -overwrite -icem mesh_file.msh -def def_file.def -ccl ccl_file.ccl

Hope this helps
  Reply With Quote

Old   August 13, 2007, 03:08
Default Re: Pre in batch mode
  #3
Kuts
Guest
 
Posts: n/a
Hello hdj,

Thanks for your response. But I have one more doubt. In fact I have more than one domains in the problem and I have them as three different meshes. How to tackle this problem. And, in the command you have suggested "-icem meshfile.msh", but can I use meshfile.cfx also, since ICEM output for CFX format is in *.cfx? Hope to hear from you..

Chao, Kuts
  Reply With Quote

Old   August 13, 2007, 09:57
Default Re: Pre in batch mode
  #4
Kuts
Guest
 
Posts: n/a
Hello All,

Can any one tell me please how to use cfx5gtmconvert command, if I need to import more than one mesh files and then write .def file from them using a ccl file. The help menu says only about one source and one Target files.

Thanks a ton, Regards Kuts
  Reply With Quote

Old   August 14, 2007, 08:54
Default Re: Pre in batch mode
  #5
CycLone
Guest
 
Posts: n/a
I wouldn't follow hdj's suggestion. Using cfx5gtmconvert in this manner will only work if the regions in your mesh file exactly correspond to your CCL state.

You can initially do the setup manually in Pre and save the physics and setup to a CCL file for re-use. Run another Pre session where you save the session file and record the actions of your script (i.e. load the grid(s), load the .ccl file, write the .def file) and quit the Pre session.

The session file (.pre) will contain the actions and the state file (.ccl) will have the physics setup. You can then run this in either line input mode or batch (line input mode allows an external script to send commands to Pre and opens a single viewer window, whereas batch mode requires a completely self contained script). If you like, you can also break the library up into snippets of physics to assemble for different cases.

If you require any additional logic, to determine what to do with non-standard boundary conditions or region names, for instance, you can add PERL programming constructs to your .pre file.

-CycLone
  Reply With Quote

Old   August 14, 2007, 14:00
Default Re: Pre in batch mode
  #6
Kuts
Guest
 
Posts: n/a
Hello Mr CycLone,

Thanks a lot for your information. Since I am bit new in using this tool, I need bit more information. I understood half what you have told and also have created .pre file.

Now my doubt is: I need to run many number of cases with different meshes (different geometries) but very same Boundary conditions. So, if I just put the new mesh in the working directory, hope while running the .pre will call the respective mesh, apply the BC and create def. And, what command I need to use if I need to run that .pre file in batch mode. I don't want to open the PRE GUI at all, since I am trying to accommodate this command in an automation loop. Hope I have made my doubt clear. Hope you can help me out here.

Thanks Kuts
  Reply With Quote

Old   August 14, 2007, 14:33
Default Re: Pre in batch mode
  #7
CycLone
Guest
 
Posts: n/a
Hi Kuts,

If you look through the .pre file you will see the line which includes the import command. If you use the same mesh filename each time, it will pick up your current mesh. You can modify the path and filename as necessary.

To run Pre in batch mode, just add the -batch flag and specify the session file name. For more flags and options, run "cfx5pre -help".

-CycLone
  Reply With Quote

Old   August 17, 2007, 05:10
Default Re: Pre in batch mode
  #8
Kuts
Guest
 
Posts: n/a
Hello Mr CycLone,

Thanks a lot for your help. It works well now.

Regards Kuts
  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


LinkBacks (?)
LinkBack to this Thread: http://www.cfd-online.com/Forums/cfx/24399-pre-batch-mode.html
Posted By For Type Date
hdjin dou - ???? This thread Refback June 3, 2015 09:35

Similar Threads
Thread Thread Starter Forum Replies Last Post
to run a replayfile in batch mode from UNIX froztbear ANSYS Meshing & Geometry 4 May 13, 2014 08:00
Running Ansys in BAtch Mode kuleuvenstudent ANSYS 0 November 5, 2010 13:27
cfdpost in batch mode taichijulie CFX 1 October 25, 2010 15:29
double precision for batch mode Lawrence STAR-CD 2 April 7, 2010 19:10
Prosurf in batch mode Dhruv CD-adapco 1 September 19, 2005 18:02


All times are GMT -4. The time now is 21:47.