[zyntbz]

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.

[Lance]

Originally Posted by zyntbz

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]

Originally Posted by Lance

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?

[Lance]

Originally Posted by zyntbz

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.

[zyntbz]

Originally Posted by Lance

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?

[Lance]

Originally Posted by zyntbz

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).

[zyntbz]

Originally Posted by Lance

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

[Lance]

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.

[zyntbz]

Originally Posted by Lance

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]

Originally Posted by zyntbz

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.