[skbme]

I use a file>export>during calculation and save output results in Ansys fluent.

However, in grid independence study, results of the iterative simulation are overwrited to the same file name.

Is there a way to parameterize filename as output parameter so that i can impose different file name?

Thank you all.

[vinerm]

You can use %i in steady-state and %t in transient case within the file name. %i and %t are replaced by iteration and time-step number, resp. If filename is firstcase.cas.gz, you should write it as firstcase_%i.cas.gz. Fluent will automatically replace %i.

[skbme]

Originally Posted by vinerm

You can use %i in steady-state and %t in transient case within the file name. %i and %t are replaced by iteration and time-step number, resp. If filename is firstcase.cas.gz, you should write it as firstcase_%i.cas.gz. Fluent will automatically replace %i.

Thank you for your kindly answer.

But what i want is that, for example, for two different meshes first mesh(coarse mesh) simulation on same fluent setting, the results file saved as follows firstcase_1.cas.gz firstcase_2.cas.gz ... according to time steps.

And for the second mesh (dense mesh) simulation, i should write filename as follows secondcase_1.cas.gz secondcase_2.cas.gz for mesh independence test.

If we have n meshes, then first ~, second_timesteps, ... n_timesteps.

so i want filename as output parameter so that i can handle it in parameter dialog like in WB.

https://www.youtube.com/watch?v=J0vRBB5yv00

[vinerm]

I am not very sure if I understand you correctly, but if you want to use an input parameter as file name, that may or may not be allowed. Better to use a journal to run the simulations and use commands with any name you want to save the files. If you are using WB, then WB will automatically name them separately, even in separate folders.

[skbme]

Originally Posted by vinerm

I am not very sure if I understand you correctly, but if you want to use an input parameter as file name, that may or may not be allowed. Better to use a journal to run the simulations and use commands with any name you want to save the files. If you are using WB, then WB will automatically name them separately, even in separate folders.

Hmm, not clear for me. what is journal? so this method can preset filename and automatically simulate multiple times in same fluent setting but different meshes?

[vinerm]

Journals are text user interface commands that can do almost everything in Fluent, such as, loading a mesh, setting up a case, running it, post processing it, saving intermediate files, almost everything barring a small part. Look at

https://www.afs.enea.it/project/nept...t/main_pre.htm

Do note that journal commands are sequential and the sequence changes from model to model, though the top level commands remain as it is. Some of these also change from version to version due to additions or subtractions from Fluent. Best approach is to press Enter in Fluent and it will show all the top level commands. Then, you can type one of these and press enter. Then it will show you second level commands and so on. All the required commands to do something can be put in a text file and read in Fluent either from File > Read > Journal or via command f r-j; f stands for file, r-j for read-journal. It expects a name of a journal file as argument. An example to load a case and data file, run it for 100 iterations (steady-state), and then save it is as follows

file read-cas-dat nameOfTheCaseFile.cas.gz
it 100
file write-cas-dat nameOfTheCaseFile_%i.cas.gz
exit y

In the above example it is assumed that the names of the case file and data file are same. If those are not, then you have to replace the first line with two following lines

f r-c caseFileName.cas.gz
f r-d dataFilename.dat.gz

Rest will be as it is.