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

Iteration number - flow rate relation

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 27, 2016, 08:49
Question Iteration number - flow rate relation
  #1
New Member
 
Join Date: Jan 2016
Posts: 5
Rep Power: 6
helvas is on a distinguished road
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.
helvas is offline   Reply With Quote

Old   May 27, 2016, 09:48
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,469
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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 is offline   Reply With Quote

Old   May 27, 2016, 09:50
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,469
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 27, 2016, 10:55
Default
  #4
New Member
 
Join Date: Jan 2016
Posts: 5
Rep Power: 6
helvas is on a distinguished road
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

Last edited by helvas; May 30, 2016 at 02:48.
helvas is offline   Reply With Quote

Old   May 28, 2016, 06:58
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,469
Rep Power: 128
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   May 30, 2016, 02:30
Default
  #6
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 669
Rep Power: 18
Lance is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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>
Lance is offline   Reply With Quote

Old   May 30, 2016, 03:57
Default
  #7
New Member
 
Join Date: Jan 2016
Posts: 5
Rep Power: 6
helvas is on a distinguished road
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.
helvas is offline   Reply With Quote

Reply

Tags
expression, flow rate, iteration, optimization

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
mass flow inlet and pressure outlet with target mass flow rate Zigainer FLUENT 13 October 26, 2018 06:58
Pressure Outlet Targeted Mass Flow Rate LuckyTran FLUENT 1 November 23, 2016 11:40
Compressor Simulation using rhoPimpleDyMFoam Jetfire OpenFOAM Running, Solving & CFD 107 December 9, 2014 14:38
DecomposePar unequal number of shared faces maka OpenFOAM Pre-Processing 6 August 12, 2010 10:01
Unaligned accesses on IA64 andre OpenFOAM 5 June 23, 2008 11:37


All times are GMT -4. The time now is 16:20.