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

Courant number

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

Like Tree3Likes
  • 1 Post By newbie384
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   March 27, 2014, 11:04
Default Courant number
  #1
Member
 
Join Date: Mar 2013
Posts: 57
Rep Power: 4
newbie384 is on a distinguished road
Hi

Some resources online say that for transient simulation, the courant number should be between 2 to 10. I think CFX reports the maximum and RMS courant number at every timestep. May I know when we say that the courant number should be between 2 to 10, is it mean the RMS courant? or the maximum courant?

Thank you in advance.
SteveNavArch likes this.
newbie384 is offline   Reply With Quote

Old   March 27, 2014, 12:25
Default
  #2
New Member
 
Stefan Hoerner
Join Date: May 2013
Posts: 5
Rep Power: 4
st_hoerner is on a distinguished road
Hello newbie,

I'm also new in cfd but this is what i understood:

it depends on your solver and discretization sheme if it is stable to calculate with co numbers>1, but even if it is stable you should check if the results become poor if you use high co numbers.

In general you can use co numbers above 1 with implict solvers but best is to keep co number <1 for good results anyway

so it is the maximum value which is interesting because it affects the calculation in the cell that is calculated with this max value.

I don't know much about cfx but with openfoam i had an effect to the results already by co>1 which kept the same value by increasing to 30...then it was getting unstable but the results were the same.

Hope this helps you..

Yours stefan
st_hoerner is offline   Reply With Quote

Old   March 27, 2014, 17:52
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,822
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I should write an FAQ on this....

CFX is an implicit solver and therefore does not have a numerical stability limit based on Courant Number. Explicit solvers do have this stability limit and are therefore strictly limited by Courant number. So Courant number is critical for Explicit solvers, and not critical for Implicit solvers.

So for implicit solvers like CFX what is the relevance of Courant Number? As always, it depends .

For most physics models which are well linearised in the solver it has little relevance. Time step size should be set by a sensitivity analysis where you vary the time step size until it gives an answer accurate to within a tolerance you are happy with.

However CFX does have some physics models which are not well linearised and they start to show explicit-like characteristics. An example of this is the surface tension model in CFX, but there are probably others. When you use these models you will find that the necessary time step size will probably drop to a Courant number near 1. But again, rather than using Courant number to set time step size I still recommend a time step sensitivity analysis.

Having said that, in general my recommendation for time step size is to use adaptive time stepping, homing in on 3-5 coeff loops per time step. This will automatically find a time step where the solver is running efficiently and small enough to be well converged for most applications.

So I do not recommend using Courant number in any form (average or max) for controlling time step size in CFX.
SteveNavArch likes this.
ghorrocks is offline   Reply With Quote

Old   March 27, 2014, 17:54
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,822
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I should point out that comparing Courant numbers between software is not very useful and they all have different implementations of the numerics, and there is little advantage in comparing Courant numbers between simulations as different simulations need different time step resolution. Hopefully by now I have convinced you Courant number is pretty useless for most applications in CFX.
SteveNavArch likes this.
ghorrocks is offline   Reply With Quote

Old   March 28, 2014, 07:14
Default
  #5
Member
 
Join Date: Mar 2013
Posts: 57
Rep Power: 4
newbie384 is on a distinguished road
hi. Thank you very much for your great explanation. So, can I say that Courant number is only valid for stability of simulation (diverge or not)? I am trying to simulate unsteady pressure at the tip of rotor due to stator-rotor interaction in centrifugal compressor and but I found that my unsteady pressure converges to a steady value as time proceeds. I wonder whether there is anything to do with the courant number or not.
newbie384 is offline   Reply With Quote

Old   March 28, 2014, 07:29
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,822
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
No, Courant number is not much use in predicting whether a CFX simulation will diverge or not either.

Using a smaller time step is a standard response to convergence difficulties. A smaller time step will also reduce the Courant number. So they go together.
ghorrocks is offline   Reply With Quote

Old   March 28, 2014, 08:52
Default
  #7
Member
 
Join Date: Mar 2013
Posts: 57
Rep Power: 4
newbie384 is on a distinguished road
Thank you for your clarification.
newbie384 is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Sudden jump in Courant number NJG OpenFOAM Running, Solving & CFD 7 May 15, 2014 13:52
Stable boundaries marcoymarc CFX 33 March 13, 2013 07:39
Courant number fireman FLUENT 4 October 4, 2010 12:54
LES near wall model & courant number kasim CFX 5 March 16, 2008 19:23
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58


All times are GMT -4. The time now is 07:41.