CFL Number

ashf9 · March 10, 2022, 13:45

Hi,

Does anyone know what the CFL number does and is it applicable to steady flow simulations. When I run my simulations I sometimes get the error saying
AMG solve rejected. CFL 216.14 -> 108.07. Would someone be able to explain to me why this is the case and what a reasonable CFL number would be for an aerofoil under stall?

Many Thanks,

fluid23 · March 10, 2022, 14:31

The steady solver uses a pseudo-time marching approach so there is still a CFL number. From the output you shared, it looks like you have the default 'automatic control' option enabled and what's happening is the solver is advancing, trying to manage your CFL number to speed up convergence. It didn't resolve the iteration at the CFL it had chosen, so it reduced it's guess and tried again.

The default limits for auto control are a little ridiculous in my opinion. I usually impose a new (lower) limit when I start seeing AML rejection repeatedly.

ashf9 · March 11, 2022, 04:14

Ah I see, thank you I've set the limit to 500, but the problem is it converges nicely for a 2D case but when I impose it on a 3D simulation with 2 slip walls, it doesn't seem to be converging, would you say I need to go lower?

Quote:

Originally Posted by fluid23

The steady solver uses a pseudo-time marching approach so there is still a CFL number. From the output you shared, it looks like you have the default 'automatic control' option enabled and what's happening is the solver is advancing, trying to manage your CFL number to speed up convergence. It didn't resolve the iteration at the CFL it had chosen, so it reduced it's guess and tried again.

The default limits for auto control are a little ridiculous in my opinion. I usually impose a new (lower) limit when I start seeing AML rejection repeatedly.

fluid23 · March 11, 2022, 09:25

The value of the CFL number shouldn't make a difference in the final result as long as it isn't so high that the solver is unstable or so low that the solver is too stiff. Poor convergence can be due to a number of things, most commonly poorly posed boundary conditions and/or poor quality mesh. I would start there in trying to track down convergence issues.

May I ask how you are judging convergence? Many people place too much emphasis on residual convergence. The 3 orders of magnitude rule that you often see quoted is a good place to start, but if you have a really good initialization, you may not get 3 orders of magnitude. I have run into this using the grid sequencing expert initialization option.

In such cases, it is helpful to consider the magnitude of the residuals, not the normalized residuals, where they are occurring in the domain, etc. You can setup your own residual monitors by turning on temporary storage and creating some plots. I have gone as far as to create separate residual plots for separate regions to help me understand what was happening with the domain.

All I am saying is, don't get hung up on residual convergence. Convergence of figures of merit (drag coefficient for example) is much, much more important. I have seen flow fields where the residual plots are converged but the things I care about in the flow are still asymptotically approaching some value.

March 10, 2022, 13:45	CFL Number	#1
ashf9 New Member Ash Join Date: Feb 2021 Posts: 20 Rep Power: 5	Hi, Does anyone know what the CFL number does and is it applicable to steady flow simulations. When I run my simulations I sometimes get the error saying AMG solve rejected. CFL 216.14 -> 108.07. Would someone be able to explain to me why this is the case and what a reasonable CFL number would be for an aerofoil under stall? Many Thanks,

March 10, 2022, 14:31		#2
fluid23 Senior Member Matt Join Date: Aug 2014 Posts: 947 Rep Power: 17	The steady solver uses a pseudo-time marching approach so there is still a CFL number. From the output you shared, it looks like you have the default 'automatic control' option enabled and what's happening is the solver is advancing, trying to manage your CFL number to speed up convergence. It didn't resolve the iteration at the CFL it had chosen, so it reduced it's guess and tried again. The default limits for auto control are a little ridiculous in my opinion. I usually impose a new (lower) limit when I start seeing AML rejection repeatedly. Last edited by fluid23; March 10, 2022 at 15:55.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
decomposePar no field transfert	Jeanp	OpenFOAM Pre-Processing	3	June 18, 2022 12:01
[snappyHexMesh] Error snappyhexmesh - Multiple outside loops	avinashjagdale	OpenFOAM Meshing & Mesh Conversion	53	March 8, 2019 09:42
[mesh manipulation] Importing Multiple Meshes	thomasnwalshiii	OpenFOAM Meshing & Mesh Conversion	18	December 19, 2015 18:57
foam-extend_3.1 decompose and pyfoam warning	shipman	OpenFOAM	3	July 24, 2014 08:14
Cluster ID's not contiguous in compute-nodes domain. ???	Shogan	FLUENT	1	May 28, 2014 15:03

March 11, 2022, 09:25		#4
fluid23 Senior Member Matt Join Date: Aug 2014 Posts: 947 Rep Power: 17	The value of the CFL number shouldn't make a difference in the final result as long as it isn't so high that the solver is unstable or so low that the solver is too stiff. Poor convergence can be due to a number of things, most commonly poorly posed boundary conditions and/or poor quality mesh. I would start there in trying to track down convergence issues. May I ask how you are judging convergence? Many people place too much emphasis on residual convergence. The 3 orders of magnitude rule that you often see quoted is a good place to start, but if you have a really good initialization, you may not get 3 orders of magnitude. I have run into this using the grid sequencing expert initialization option. In such cases, it is helpful to consider the magnitude of the residuals, not the normalized residuals, where they are occurring in the domain, etc. You can setup your own residual monitors by turning on temporary storage and creating some plots. I have gone as far as to create separate residual plots for separate regions to help me understand what was happening with the domain. All I am saying is, don't get hung up on residual convergence. Convergence of figures of merit (drag coefficient for example) is much, much more important. I have seen flow fields where the residual plots are converged but the things I care about in the flow are still asymptotically approaching some value.