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

continuing to solution

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

Like Tree1Likes
  • 1 Post By Lance

Reply
 
LinkBack Thread Tools Display Modes
Old   June 27, 2011, 03:32
Default continuing to solution
  #1
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
zyntbz is on a distinguished road
Hello everybody,
I've been working with Ansys-CFX about a transient heat transfer problem. I start to solve a problem and it takes at least 5 or more days (sometimes a month). If there's any trouble in computer system or the electircity (when computer shuts down or something..) I cannot get the result file and I have to start to the solution over! And it's just the waste of time! When I look at the working folder, there are trn. files. Can I use these trn files and continue to the solution from the time last trn file being created.
zyntbz is offline   Reply With Quote

Old   June 27, 2011, 04:24
Default
  #2
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 540
Rep Power: 11
Lance is on a distinguished road
Quote:
Originally Posted by zyntbz View Post
Hello everybody,
Can I use these trn files and continue to the solution from the time last trn file being created.
Yes, trn files are the results files from a transient solution and you can normally restart a solution from them.
zyntbz likes this.
Lance is offline   Reply With Quote

Old   June 27, 2011, 06:15
Default the procedure
  #3
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
zyntbz is on a distinguished road
Quote:
Originally Posted by Lance View Post
Yes, trn files are the results files from a transient solution and you can normally restart a solution from them.
Thank you for reply. Do you know how to continue to solution from the created trn files? I mean which procedure I should follow?
zyntbz is offline   Reply With Quote

Old   June 27, 2011, 06:46
Default
  #4
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 540
Rep Power: 11
Lance is on a distinguished road
Quote:
Originally Posted by zyntbz View Post
Thank you for reply. Do you know how to continue to solution from the created trn files? I mean which procedure I should follow?
This is discussed in the manual, but here goes:

In the solver manager:
Initial values specification/File Name: "your last .trn file"
Continue history from: initial values

or, using the command line
cfx5solve -def $deffile -continue-from-file $inifile
where $deffile and $inifile is defined as your definition file and trn file, respectively.
Lance is offline   Reply With Quote

Old   June 27, 2011, 08:06
Default doesn't work
  #5
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
zyntbz is on a distinguished road
Quote:
Originally Posted by Lance View Post
This is discussed in the manual, but here goes:

In the solver manager:
Initial values specification/File Name: "your last .trn file"
Continue history from: initial values

or, using the command line
cfx5solve -def $deffile -continue-from-file $inifile
where $deffile and $inifile is defined as your definition file and trn file, respectively.
Thank you for your reply,
I can't use these steps. I already tried this way, but the computer didn't restart normally.. It gives following error message and doesn't start to solve;

''the simulation terminated with errors. run concluded at Mon 27. No results are available!''

So I've been solving the problems which takes long time (1 month or more) by seperating the time. For example if I have 120 seconds run, I solve the problem with 10 sec parts.

But I couldn't get a solution any further than that! If you have any suggestion, I'd be happy?
zyntbz is offline   Reply With Quote

Old   June 27, 2011, 08:13
Default
  #6
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 540
Rep Power: 11
Lance is on a distinguished road
Quote:
Originally Posted by zyntbz View Post
It gives following error message and doesn't start to solve;

''the simulation terminated with errors. run concluded at Mon 27. No results are available!''
This error message is useless, it doesnt tell us anything about what went wrong. Post the error message in the output from the solver instead (look in a file called "something"_001.out).
Lance is offline   Reply With Quote

Old   June 28, 2011, 07:06
Default the file
  #7
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
zyntbz is on a distinguished road
Quote:
Originally Posted by Lance View Post
This error message is useless, it doesnt tell us anything about what went wrong. Post the error message in the output from the solver instead (look in a file called "something"_001.out).
I tried to use .trn files insted of result file. it didn't work.We get this error text. Here's the error message:
error .txt
zyntbz is offline   Reply With Quote

Old   June 28, 2011, 07:14
Default
  #8
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 540
Rep Power: 11
Lance is on a distinguished road
Thats all? Error creating namemap: G/BCS missing ?

Two things:
When you are saving the .trn files, do you only save a few selected variables or "standard". If you only save, say, temperature and HTC then the trn file does not contain enough data for a restart and it will fail. Could this be the issue?

Also, avoid spaces in folder and file names.
Lance is offline   Reply With Quote

Old   June 28, 2011, 09:50
Default save backup
  #9
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
zyntbz is on a distinguished road
Quote:
Originally Posted by Lance View Post
Thats all? Error creating namemap: G/BCS missing ?

Two things:
When you are saving the .trn files, do you only save a few selected variables or "standard". If you only save, say, temperature and HTC then the trn file does not contain enough data for a restart and it will fail. Could this be the issue?

Also, avoid spaces in folder and file names.
Yes I only select a few variables such as Temp, velocity, vorticity.
But I guess there's another way. I use the 'save backup file' option while the simulation's running. Therefore I can use this backup file as a result file, and continue to the solution from the intermediate time. But choosing all the variables may help.

I'll write if it works.Thank you.
zyntbz is offline   Reply With Quote

Old   June 28, 2011, 10:53
Default it works!
  #10
New Member
 
Join Date: Mar 2011
Posts: 6
Rep Power: 6
zyntbz is on a distinguished road
Quote:
Originally Posted by zyntbz View Post
Yes I only select a few variables such as Temp, velocity, vorticity.
But I guess there's another way. I use the 'save backup file' option while the simulation's running. Therefore I can use this backup file as a result file, and continue to the solution from the intermediate time. But choosing all the variables may help.

I'll write if it works.Thank you.
choosing the standard option solved the error problem. I can use the trn files by choosing standard results in the output controls.

Thank you.
zyntbz 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
Integrated conjugate heat transfer solver in OpenFOAM hjasak OpenFOAM Running, Solving & CFD 168 June 27, 2013 01:56
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
solution singularity litonx OpenFOAM Running, Solving & CFD 1 February 21, 2007 02:32
Mesh independent solution CFX Begineer CFX 0 October 27, 2002 11:54
Discussion about Mesh independant solution Seb Main CFD Forum 13 May 22, 2001 13:37


All times are GMT -4. The time now is 03:54.