CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   CFL number (http://www.cfd-online.com/Forums/cfx/19826-cfl-number.html)

Daniele August 12, 2003 02:12

CFL number
 
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.

Reemull August 12, 2003 04:52

Re: CFL number
 
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

Ben August 12, 2003 08:13

Re: CFL number
 
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

Glenn Horrocks August 12, 2003 18:17

Re: CFL number
 
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

Mina_Shahi July 19, 2012 09:46

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.

ghorrocks July 19, 2012 19:11

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.


All times are GMT -4. The time now is 02:47.