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

CFL number

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 12, 2003, 02:12
Default CFL number
  #1
Daniele
Guest
 
Posts: n/a
Hi, I have a problem with a transient simulation in cfx –Tascflow. In the out-file there is a notice about the CFL number. It's too big. I'd like to know if this can be a problem for the results of the simulation. Thanks a lot.
  Reply With Quote

Old   August 12, 2003, 04:52
Default Re: CFL number
  #2
Reemull
Guest
 
Posts: n/a
Yes it can. There are other threads around which explain more about the CFL number, however the CFL number is a function of your solution timestep and the grid size. For a transient simulation the CFL number must be less than 1.

In the out file it should tell you what your largest CFL number is. Divide your timestep by a number just slightly bigger than the CFL number in your outfile and this should drop the CFL number below 1.

So if your out file said your largest CFL number was 35, I'd divide the present timestep by 36 to gain the new timestep and rerun. This would drop the CFL number below 1 and remove the notice in the out file.

Hope this helps

Roy
  Reply With Quote

Old   August 12, 2003, 08:13
Default Re: CFL number
  #3
Ben
Guest
 
Posts: n/a
Hi Roy!

I have got a similar problem as Daniele has. I want to investigate the transient behaviour of an annular seal by using the moving grid feature in CFXTascflow. Now i always get the information that the CFL- Number is bigger than 1 at 100% of the nodes. The CFL-number is even too big to display the value. I only get eight * instead of the true value.

My problem is that i can not reduce the timestep as much as a should because of the resulting big effort in calculation time (Moving Grid is only available for serial computing). I also can not generate a coarser grid because of the yplus-value. (i am interested in friction losses which result).

But if i compare the simulated results with measuring points than i can see that they are nearly coincident. Now i am not sure whether i can thrust this simulation or not.

Please, can anybody help me and give me some guidance.

Ben
  Reply With Quote

Old   August 12, 2003, 18:17
Default Re: CFL number
  #4
Glenn Horrocks
Guest
 
Posts: n/a
Hi Reemull,

I do not know Tascflow at all (I am a CFX5 man), but they use the same basic solver technique so hopefully what I am about to say is still accurate.

The solver is not restricted to a maximum CFL of 1. The CFL<=1 restriction applies to explicit solvers, and CFX/Tascflow is implicit and does not have this restriction. The maximum CFL number you can run is problem dependent, but in my experience in simple compressible flows (eg shock tube) you can run maximum CFL to between 10 and 50. However when the Mach number starts to get high (over 2) the maximum CFL will come down closer to one. Simple flows with little gas compression (eg Mach<0.3) can go even higher. Things which really start limiting the size timestep you can run include combustion and free surfaces.

I recommend doing a timestep independence test and really finding out what timestep you need. This is an essential part of the validation of any transient CFD simulation.

Glenn
  Reply With Quote

Old   July 19, 2012, 09:46
Default
  #5
Member
 
Mina
Join Date: Apr 2011
Posts: 88
Rep Power: 7
Mina_Shahi is on a distinguished road
Quote:
Originally Posted by Glenn Horrocks
;67049
Hi Reemull,

I do not know Tascflow at all (I am a CFX5 man), but they use the same basic solver technique so hopefully what I am about to say is still accurate.

The solver is not restricted to a maximum CFL of 1. The CFL<=1 restriction applies to explicit solvers, and CFX/Tascflow is implicit and does not have this restriction. The maximum CFL number you can run is problem dependent, but in my experience in simple compressible flows (eg shock tube) you can run maximum CFL to between 10 and 50. However when the Mach number starts to get high (over 2) the maximum CFL will come down closer to one. Simple flows with little gas compression (eg Mach<0.3) can go even higher. Things which really start limiting the size timestep you can run include combustion and free surfaces.

I recommend doing a timestep independence test and really finding out what timestep you need. This is an essential part of the validation of any transient CFD simulation.

Glenn

Hi Glenn

Do you have any documentation prove that for CFX , CFL number is not restricted? i am modeling acoustic in a chamber, my CFL number is usully higher than one, and always there is discussion about that, i would be very helpfull if you suggest me some documendation about that.
Mina_Shahi is offline   Reply With Quote

Old   July 19, 2012, 19:11
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,834
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Wow, digging up a 9 year old thread. That's going back a way...

CFX is an implicit solver, and implicit solvers do not have a strict CFL restriction, rather it is discretisation error which sets the time step size. This is basic numerical analysis and any numerical analysis textbook will confirm this.

But some sub-models in CFX have explicit components - surface tension being one I am familiar with. If you have surface tension in your model then it will start restricting the time step size. But the restriction will not be to CFL, but to some function of the surface tension state.
ghorrocks 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
SnappyHexMesh for internal Flow vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 24 June 27, 2016 08:54
external flow with snappyHexMesh chelvistero OpenFOAM 11 January 15, 2010 20:43
CFL number specification sonic/supersonic flow gr Main CFD Forum 0 January 16, 2009 12:14
high cfl number and discretization scheme Fab Main CFD Forum 0 March 2, 2008 13:19
About Courant (CFL) number Jason Main CFD Forum 2 March 17, 2003 12:11


All times are GMT -4. The time now is 20:46.