# wrong solution at LOW CFL number

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

 May 8, 2020, 10:31 wrong solution at LOW CFL number #1 Member   ARAVIND SRIDHARA Join Date: Jan 2017 Posts: 32 Rep Power: 8 I am using the k-w model for turbulence and I am solving a problem involving 3 annular jets. I use the coupled model and second-order discretization scheme for pressure and other variables. I use a default courant number of 200 and the solution converged. However, the paper that I am validating solved the problem using the Hybrid RANS-LES scheme using open foam having courant number of 0.8. I have the following doubts 1. Does courant number depends on grid 2. Does the courant number depend on type of turbulence model and solution strategy? (That is coupled solver) 3. If i decrease my CFL number below 10 my solution is not stable and I am getting reversed flow at outlet which is incorrect. I would like to know why the residuals wont convegre for low CFL number

 May 8, 2020, 12:38 Courant Number #2 Senior Member     Vinerm Join Date: Jun 2009 Location: Nederland Posts: 2,946 Blog Entries: 1 Rep Power: 34 The Courant number used in Coupled solver is not CFL criterion. Default value is 200 and you can use higher (1000s of times higher) or lower values, however, a value as low as 10 does not make sense. If case can converge with a value of 10, then even SIMPLE will work. Just use a higher value or enable Pseudo-Transient. That is more stable. __________________ Regards, Vinerm PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.

 May 8, 2020, 15:24 #3 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,149 Rep Power: 61 Already answered by vinern but I'm going to repeat it anyway just to be clearer There is no "CFL number." Quit making up terms. You only confuse yourself. Use the words on the screen. Courant number does depend on the grid. The Flow Courant number in the COUPLED P-V solver is a type of under-relaxation. High Flow Courant numbers means you converge faster. If you set super low Flow Courant numbers, you need many more iterations to converge per time-step. I like to use 2e7 for the Flow Courant number so it converges in 1 iteration like PISO. Regardless of what number you set the Flow Courant number to, it doesn't affect your Courant number (which is determined by your grid and time-step size).

 May 11, 2020, 02:55 #4 Member   ARAVIND SRIDHARA Join Date: Jan 2017 Posts: 32 Rep Power: 8 I now understood the difference between flow courant number and the actual courant number. However, I would like to know the maximum and minimum limits of my cell courant number. I have seen that we can see this in histogram plot under the velocity function. However, it is not visible in my case. I am using Ansys Fluent 16.0 . Is there any other way to see cell courant number?

 May 11, 2020, 03:02 #5 Senior Member   Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,149 Rep Power: 61 Can you make a contour plot of the Courant number? The same way you would make a pressure plot, etc? The Courant number is a field available for all unsteady solvers. I'm not sure why you're not able to see it. There isn't anything fancy you have to do.

 May 12, 2020, 10:27 #6 Member   ARAVIND SRIDHARA Join Date: Jan 2017 Posts: 32 Rep Power: 8 I am solving steady state problem not unsteady

 Tags cfl, courant number, courant number limit