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

CFX Timescale: Difference between Physical,Local facotr and Auto Timescale

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

Like Tree4Likes
  • 3 Post By Antanas
  • 1 Post By Antanas

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 6, 2014, 20:36
Default CFX Timescale: Difference between Physical,Local facotr and Auto Timescale
  #1
Member
 
Faizan
Join Date: Mar 2014
Posts: 76
Rep Power: 12
Mfaizan is on a distinguished road
Hi all,

Please suggest me the difference between Physical timescale, Local timescale factor and Auto timescale?

first I tried my cfd project with auto timescale, then local timescale factor and then physical timescale.

The problem I am having with physical timescale is that it is finishing before the suggested iterations. I set 1000 iterations but with physical timescale the solver stopped after 141 iterations. WHY? I do not understand. Please anyone know the reason then please reply to this post............Humble request.....

Thanks in advance
Mfaizan is offline   Reply With Quote

Old   April 7, 2014, 01:06
Default
  #2
Senior Member
 
Join Date: Feb 2011
Posts: 496
Rep Power: 18
Antanas is on a distinguished road
Quote:
Originally Posted by Mfaizan View Post
Hi all,

Please suggest me the difference between Physical timescale, Local timescale factor and Auto timescale?
Physical timescale - you set fixed time scale to be used over the entire flow domain;

Auto timescale - CFX determines time step automatically based on the boundary conditions, flow conditions, physics, and domain geometry;

Local timescale factor - enables different time scales to be used in different regions of the calculation domain. The value you enter is a multiplier of a local element-based time scale.

Why don't you use CFX help?

Quote:
Originally Posted by Mfaizan View Post
The problem I am having with physical timescale is that it is finishing before the suggested iterations. I set 1000 iterations but with physical timescale the solver stopped after 141 iterations. WHY? I do not understand. Please anyone know the reason then please reply to this post............Humble request.....

Thanks in advance
It doesn't related to physical timescale. The solver finishes either when convergence criteria (residuals target, conservation target (imbalances)) are met or when max number of iterations are reached. Max number of iterations is just limiter. If solver finishes before max number of iteration then it means that your residuals became less than residual target and your imbalances are less than 1% (if you activated conservation target checkbox in solver control).
hamidciv, Mfaizan and melihozgur like this.
Antanas is offline   Reply With Quote

Old   April 7, 2014, 01:10
Default
  #3
Member
 
Faizan
Join Date: Mar 2014
Posts: 76
Rep Power: 12
Mfaizan is on a distinguished road
Thanks Antanas,

What do u suggest that which timescale shud I use for my model.

I am modelling a supersonic convergent-divergent nozzle. The gas in nozzle is nitrogen with 1.4MPa total pressure and 550C total temperature inlet boundary condition.

I enclosed the nozzle in cylindrical surrounding domain filled with nitrogen gas too with opening boundary condition.

Please suggest if physical timescale is OK with my entire flow domain.
Mfaizan is offline   Reply With Quote

Old   April 7, 2014, 01:39
Default
  #4
Senior Member
 
Join Date: Feb 2011
Posts: 496
Rep Power: 18
Antanas is on a distinguished road
Quote:
Originally Posted by Mfaizan View Post
Thanks Antanas,

What do u suggest that which timescale shud I use for my model.

I am modelling a supersonic convergent-divergent nozzle. The gas in nozzle is nitrogen with 1.4MPa total pressure and 550C total temperature inlet boundary condition.

I enclosed the nozzle in cylindrical surrounding domain filled with nitrogen gas too with opening boundary condition.

Please suggest if physical timescale is OK with my entire flow domain.
My suggestions:
1. Use auto-timescale.
2. Set appropriate initial distribution. It's more important IMO. You may use gas-dynamic functions for that.
3. Use Upwind scheme to get approximate solution.
4. Use results of step 3 as initial guess and set High Resolution scheme to get final results.

You may try to use dt = C * dl / (abs(u)-a), where C <= 1, dl - smallest mesh element dimension, u - characteristic streamwise velocity component, a - characteristic speed of sound.
Mfaizan likes this.
Antanas is offline   Reply With Quote

Old   April 7, 2014, 02:03
Default
  #5
Member
 
Faizan
Join Date: Mar 2014
Posts: 76
Rep Power: 12
Mfaizan is on a distinguished road
Thanks Antanas,

Such a comprehensive response.

Sure I would try as u instructed.

Cheers,
Mfaizan is offline   Reply With Quote

Reply

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



All times are GMT -4. The time now is 22:25.