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

interpolate with batch file

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 19, 2007, 16:46
Default interpolate with batch file
  #1
Claudia
Guest
 
Posts: n/a
Hi,

I would like to interpolate the values from a file name test.res on the mesh from the file named solve.def. I would like to use the command line. In the manual there is something written like -interpolate-iv But when I write:

cfx5solve -def solve.def -interpolate-iv test.res ...and so on, it doesn't work. So, what's wrong?

Thanks

Claudia
  Reply With Quote

Old   June 19, 2007, 18:08
Default Re: interpolate with batch file
  #2
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Try cfx5interp.

Glenn Horrocks
  Reply With Quote

Old   June 20, 2007, 03:30
Default Re: interpolate with batch file
  #3
Claudia
Guest
 
Posts: n/a
Hi Glenn,

this is what i don't want, because I would like to interpolate and start the job in one step, because I am a user of a cluster and I wait a long time to start one job. So I had wo wait for the interpolation and again for the solver run. So can you tell me how the -interpolate-iv command works?

thanks
  Reply With Quote

Old   June 20, 2007, 05:25
Default Re: interpolate with batch file
  #4
michel
Guest
 
Posts: n/a
Hi Claudia,

The following works for me:

cfx5solve -batch -def solve.def -ini test.res

And edit your .def file to include: EXECUTION CONTROL: RUN DEFINITION:

Interpolate Initial Values = yes END END

You can add this manually to your .def file, or use the -ccl argument.

Regards, Michel
  Reply With Quote

Old   June 20, 2007, 05:38
Default Re: interpolate with batch file
  #5
Claudia
Guest
 
Posts: n/a
Hi Michael,

thanks for the answer, but the -ini switch only works if you have an equal mesh. I need the -interpolate command, because I have different meshs.

Or is this command from you: ... Interpolate Initial Values = yes END END ...

for interpolating on a different mesh?

Thanks Claudia

  Reply With Quote

Old   June 20, 2007, 06:52
Default Re: interpolate with batch file
  #6
Johnson
Guest
 
Posts: n/a
Hi,

when you say 'it doesn't work' do you mean that it fails, or that the job proceeds but the interpolation doesn't happen?

I think the syntax of the command you need should be

cfx5solve -def <def> -ini <res> -interp-iv ...

Is this what you are specifying?

Regards,

Johnson
  Reply With Quote

Old   June 20, 2007, 06:54
Default Re: interpolate with batch file
  #7
Johnson
Guest
 
Posts: n/a
sorry that should be

cfx5solve -def file.def -ini file.res -interp-iv ...
  Reply With Quote

Old   June 20, 2007, 07:24
Default Re: interpolate with batch file
  #8
michel
Guest
 
Posts: n/a
Sorry, the formatting got a bit screwed up before.

Indeed, "-ini test.res" only specifies that the flow solution from test.res should be used as initial guess. And for some reason CFX then also takes the mesh from test.res, not the one specified in the .def file. By adding the following CCL commands: EXECUTION CONTROL: RUN DEFINITION:

Interpolate Initial Values = yes END END

the flow solution from test.res will be interpolated onto the mesh in solve.def. Perhaps the argument -interp-iv should work, but I don't find it in the solver documentation.

Michel

  Reply With Quote

Old   June 20, 2007, 07:34
Default Re: interpolate with batch file
  #9
michel
Guest
 
Posts: n/a
Another go at decent formatting:

EXECUTION CONTROL:

RUN DEFINITION:

Interpolate Initial Values = yes

END

END

  Reply With Quote

Old   June 20, 2007, 09:05
Default Re: interpolate with batch file
  #10
Claudia
Guest
 
Posts: n/a
Dear Johnson and Michel,

thanks for the help. The command:

cfx5solve -def file.def -ini file.res -interp-iv ...

works! My problem was, that the -ini file.res was missing. I only used -interp-iv file.res that was wrong. I will test the modification in .ccl at another time, but I think that it is also a good way.

Thanks for all! Claudia
  Reply With Quote

Old   June 20, 2007, 23:32
Default Different meshes?
  #11
Stu
Guest
 
Posts: n/a
Just a clarification, you mentioned different meshes. Are they substantially different, or is one simply a scaled version of the other. The reason i am asking is that I thought you could not change the mesh that much, eg the number of boundary conditions, the connection of the nodes to form elements etc.

Is it possible to do the following. I have a small rectangular tank, and I run a multiphase sim that fills the tank with water to 50% full. I then increase the height of the tank by 20% and remesh it. Can I interpolate the previous transient results onto the new mesh as the inital values, ie the new height part of the tank would contain only air, not water. ps I dont not care about what the air is doing, only the flowing of the water.

Thanks Stu

  Reply With Quote

Old   June 21, 2007, 04:57
Default Re: Different meshes?
  #12
Johnson
Guest
 
Posts: n/a
Stu,

the interpolation should be successful - the overlap will contain the correctly interpolated solution from the previous results file, and the 'new' part should have an approximate solution based on near/surrounding nodes.

However, you should probably check the interpolated solution before embarking on the new transient analysis.

Johnson
  Reply With Quote

Old   June 21, 2007, 06:17
Default Re: Different meshes?
  #13
stu
Guest
 
Posts: n/a
Thanks for your response.

Where in the documentation does it mention

cfx5solve -def file.def -ini file.res -interp-iv ... ,

specifically the -interp-iv part. I have gone through the solver manual and connot see it in there.

Question how do I check the interpolated results, do I just run the sim for 1 more time step and then examine the results?

Thanks Stu

  Reply With Quote

Old   June 21, 2007, 08:30
Default Re: Different meshes?
  #14
KB
Guest
 
Posts: n/a
You'll find this option in the command line documentation, i.e. try

cfx5solve -h

  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
GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM 300 October 29, 2014 19:00
2.0.x on Mac OSX niklas OpenFOAM Installation on Windows, Mac and other Unsupported Platforms 74 March 28, 2012 16:46
channelFoam for a 3D pipe AlmostSurelyRob OpenFOAM 3 June 24, 2011 13:06
Version 15 on Mac OS X gschaider OpenFOAM Installation 120 December 2, 2009 11:23
gcc and executable file from Mac to Linux simone Marras Main CFD Forum 0 April 8, 2007 15:49


All times are GMT -4. The time now is 18:05.