[helvas]

Hi all,

I'm trying to observe behavior of a wing due to the different flow rates, so that i need to solve different working conditions. I start my calculations but when the analysis has completed, for every working conditions i go back to setup and changing flow rate and start again, because of that i can not leave PC alone. My analysis converging about 60-70 iterations so i think that if i change my flow rate due to iteration number, i can calculate more than one situation and i can read values from solver manager graph.

I tried to write an expression but i couldn't figure out how to write for such that problem. (Probably because i'm new on CFD (Really new!!)) Can anyone help me? or show me a way?

I need to change my flow rate based on iteration number. For example;

iteration number 0 to 100 => flow rate = 2 [kg s^-1]
iteration number 100 to 200 => flow rate = 3 [kg s^-1]
iteration number 200 to 300 => flow rate = 4 [kg s^-1]
.
.
.

and goes on.

thanks in advance and sorry for my english.

[ghorrocks]

This sounds like a really bad idea to me. A CFD simulation should progress to convergence and produce a single result. There are many different ways to get runs to queue up and run automatically and it is really easy to do:

* Batch/script file - the change to the conditions can be done by a CCL file written to the definition file by the command line cfx5cmds. Then start the run with cfx5solve. Then repeat for all the combinations you want to do.
* Use the parametric modelling in workbench
* Use a batch scheduling system like PBS, LSF (OK, this is not such a simple approach - I suspect if you used these systems you would not be asking this question But the other two options are very simple)

[ghorrocks]

Here's an example batch file which would do it:

cfx5cmds -def <def file> -text <CCL file 1>
cfx5solve -def <def file>
cfx5cmds -def <def file> -text <CCL file 2>
cfx5solve -def <def file>
cfx5cmds -def <def file> -text <CCL file 3>
cfx5solve -def <def file>

This will do 3 runs, one after the other (so only using a single license at any time) using 3 different setup CCL files.

[helvas]

Thanks a lot Glenn,
it's also seems to a stupid idea but as i told i'm very new about CFD, i will try to solve as you suggest

i also find a solution which i try to do, here is the link for anyone who needs

http://www.padtinc.com/blog/the-focu...essions-part-4

[ghorrocks]

Putting ramping or stepping functions in CEL is very useful and it is good you have a tutorial on it. But using it as a method of doing multiple simulations in a single simulation is not wise. I did not answer the question on ramping the CEL as a case of the XY problem (http://xyproblem.info/) - the real issue is how do you effectively run multiple simulations.

[Lance]

Originally Posted by ghorrocks

Here's an example batch file which would do it:
cfx5cmds -def <def file> -text <CCL file 1>
cfx5solve -def <def file>
cfx5cmds -def <def file> -text <CCL file 2>
cfx5solve -def <def file>
cfx5cmds -def <def file> -text <CCL file 3>
cfx5solve -def <def file>

I agree with Glenn that it is a bad idea to ramp flow rates with iteration number. Use a batch file instead, but there is no need to modify the -def file, you can specify the ccl file directly in the cfx5solve command as
cfx5solve -def <def file> -ccl <CCL file 1>
cfx5solve -def <def file> -ccl <CCL file 2>
cfx5solve -def <def file> -ccl <CCL file 3>

[helvas]

Dear Glenn, Lance;

Thank you for advices, I made a search for parametric modelling and Batch/script file, and using parametric modelling seems to me very easy and i prepared my setup parametric. I have solution now, thank you very much.