CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM Running, Solving & CFD (
-   -   How to choose the right courant number? (

vitor October 28, 2009 14:23

How to choose the right courant number?
How to choose the right Courant number in complexes simulations (3D, with a great number of cells) and what are its implications?


MadsR October 29, 2009 04:50

Hi Vitor.

The Courant/CFL number (wiki here) depends, as you probably know, on velocity, cell-size and time step and is typically calculated for each cell. The Courant number will accordingly change a bit with velocity when you have a static mesh and a constant time step. Now, assuming here that your mesh is static (non-moving/morphing) and that the velocity field is more or less fully developed, changing the time step is a good way of controlling the Courant number.

A physical explanation, for a CFD simulation, of the Courant number could be that it tells you something about how fluid is moving through your computational cells. If the Courant number is <=1 fluid particles move from one cell to another within one time step (at most). If it is >1 a fluid particles moves through two or more cells at each time step and this can affect convergence negatively. Robust systems and fine solvers, as OpenFOAM, easily deals with large Courant numbers way into the houndreds, but it's a good place to look if you have Convergence problems and it also can effect accuracy of a transient simulation. Diffusion dominated problems should typically be run with low Courant numbers, if I remember correctly.

Hope it helps you a bit, I didn't mean to lecture you if you already knew this.

Short answer is: lower time step to lower Courant number, raise time step to increase Courant number.


akidess October 29, 2009 12:46

For complex simulations with changing velocities it can help to use automatic time step adjustment. See how it's implemented in the interFoam solver (, or also threads in the forum (e.g. Problems with adjustable timestep control and maxCo Number).

vitor October 30, 2009 06:23


Originally Posted by akidess (Post 234532)
For complex simulations with changing velocities it can help to use automatic time step adjustment. See how it's implemented in the interFoam solver (, or also threads in the forum (e.g. Problems with adjustable timestep control and maxCo Number).

I've seen it, but do you have any tips for setting the right maxCo?



akidess October 30, 2009 15:10

Unfortunately I don't think there is a general recipe for that. You will have to play around a little and see what works for you. As Mads already lined out, maxCo will usually have to be smaller than 1, and I think you will rarely have to make it smaller than 0.5. April 24, 2010 20:02

I think that the best approach is to make different simulations with decreasing values of the time step until the final solution becomes independent of this value. I have already made some simulations where the maximum Courant was of the order of hundreds and, nevertheless, the solution was already converged.

dohnie April 27, 2010 05:31

Actually, in compressible flow (if you are interested in acoustic waves or shocks) the courant number should not be based on velocity U, but on U+a (sound speed).
Does anybody know if this is implemented in OpenFOAM? Seems to be trickier than I thought at first, because U is a volVectorField and a is a volScalarField (thus it should always be added in the positive U-direction).

SMesser April 28, 2011 17:48

adjustable time step doesn't limit Courant?
I'm using sonicDyMFoam with a solid object moving through a confined space (a fast gas valve). I'm getting lots of trouble with "max number of iterations exceeded" in the calculation of e and "time step continuity errors". I've tried setting maxCo=0.2 and maxAlphaCo=0.2 in system/controlDict, yet the text output shows the max Courant number is still sometimes 1 or larger... sometimes the mean is >1 as well.

Is this normal? my controlDict is as follows:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.7.1                                |
|  \\  /    A nd          | Web:                      |
|    \\/    M anipulation  |                                                |
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "system";
    object      controlDict;
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application    sonicDyMFoam;

startFrom      startTime;

startTime      0;

stopAt          endTime;

endTime        0.001;

deltaT          1e-7;

writeControl    adjustableRunTime;

writeInterval  1e-6;//2e-5

purgeWrite      0;

writeFormat    ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision  6;

runTimeModifiable yes;

adjustTimeStep  yes;

maxCo          0.2;
maxAlphaCo      0.2;

maxDeltaT      1;

// ************************************************************************* //


maysmech April 30, 2011 08:58

I have this problem too.

I can't use max courant setting for pisoFoam and simpleFoam.

Any suggestion?


truong_nm May 2, 2011 04:39

CFL in steady solvers
Hi maysmech,

There's no CFL Number in such steady solvers. In OF, steady solver means "d/dt=0". Thus, there is no more time step and so no more Courant Number.

I do agree with you: how to control stability in such cases?
The answer is: relaxation factors.


maysmech May 2, 2011 06:23

You right, I meant pisoFoam only. It is an unsteady solver.

SMesser May 4, 2011 13:35

details of crash
A couple of updates - I tried increasing the spatial and temporal resolution to get y+ to about 63, following the Best-Practices for TurboMachinery page on the CFD Wiki, but the sim crashed _faster_... which seems odd. I'm dealing with a fast-opening gas valve. (40 psi Argon on one side, vacuum on the other; device spatial scales are on the order of 1 cm, and opening time is measured in several tens of microseconds.) I also found a web tutorial with info on revising OpenFoam codes to do adaptive timesteps, but it seemed fairly out-of-date and led to me reinstalling OpenFoam. (I'm missing some library; compilation fails unless I'm in the midst of the install.)

I've learned a couple other things:
1) Strong pressure differences (or maybe just strong gradients?) cause crashiness, but I'm not sure _why_ or if there's a workaround. I changed the "vacuum" to 10 psi to avoid the problem, but the motion of the valve's poppet still generates a near-vacuum for some time. (The mechanical parts move slower than Mach 1, but the gas still has to flow supersonically to fill in the gaps through narrow channels.)

2) non-convergence seems to show up at calculation of either e or T. This makes me think my problem's in the choice of thermodynamic model (currently

thermoType      ePsiThermo<pureMixture<constTransport<specieThermo<hConstThermo<perfectGas>>>>>;
), but I'd love feedback from someone with more experience

3) The message from the last timestep is

Time = 5.68e-06

Courant Number mean: 0.000260452 max: 0.850669
DICPCG:  Solving for cellMotionUx, Initial residual = 1.7015e-07, Final residual = 9.6024e-09, No Iterations 80
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 0.641902, Final residual = 4.55875e-06, No Iterations 3
DILUPBiCG:  Solving for Uy, Initial residual = 0.0790439, Final residual = 2.72074e-07, No Iterations 4
DILUPBiCG:  Solving for e, Initial residual = 0.967212, Final residual = 6.18915e-06, No Iterations 2

Maximum number of iterations exceeded

    From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
    in file /home/opencfd/OpenFOAM/OpenFOAM-1.7.x/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 67.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam171/lib/linuxGccDPOpt/"
#1  Foam::error::abort() in "/opt/openfoam171/lib/linuxGccDPOpt/"
#2  Foam::ePsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::calculate() in "/opt/openfoam171/lib/linuxGccDPOpt/"
#3  Foam::ePsiThermo<Foam::pureMixture<Foam::constTransport<Foam::specieThermo<Foam::hConstThermo<Foam::perfectGas> > > > >::correct() in "/opt/openfoam171/lib/linuxGccDPOpt/"
 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/sonicDyMFoam"
#5  __libc_start_main in "/lib/"
 in "/opt/openfoam171/applications/bin/linuxGccDPOpt/sonicDyMFoam"

I'm not sure how / if I should try to increase the max number of iterations. Would it be better to increase tolerance and/or relTol in fvSchemes? T isn't directly listed there, but most listed items are at tolerance of 10^-5 or 10^-8, with relTol=0. Using relTol seems sketchy since this is a transient sim, not steady-state. Again, it'd be nifty to get feedback from an expert.

Thanks for answering the new-B questions. This isn't my first simulation, but I'm much more used to wiring up hardware than to trying to simulate its operation.

dancfd May 22, 2012 21:54

Hello Sarah,

I do not think that adjustTimeStep works for sonicDyMFoam - my experience has shown that regardless of what I set maxCo to, the timestep will revert to what I set in the deltaT field in controlDict. Granted, I am using sonicFoam vice sonicDyMFoam, however they probably have that limitation in common.

I suggest that you may have to try reducing your deltaT until you compute a Co that is where you want it to be. I find ~0.5 to be the maximum that will converge. Please post the results / let me know if you were able to resolve your issue, since I am still struggling with this too.



zaynah04 January 9, 2013 15:55

dear Mads,

i have very low courant numb 1e-5, and my solution does not acheive convergence.. can you please tell me what may be the problem?
i am using incompresible flow in laminar regime with very low velocity..

MadsR January 10, 2013 04:10

Dear Zaynah,

troubleshooting convergence problems can be easy or very, very hard, especially through a forum :)
You don't reveal enough information for anyone to help you out I think. I think that a Courant number of 1e-5 is surprisingly low (actually I would bluntly call it: way too low) but it could depend on some strange :) simulation that you are trying to perform.
Tell us more, but my intuition says that it is not your Courant number which is the problem. It seems that you have tried to lower the time step much to achieve convergence? Is it some explosion simulation or what?

best regards

Traib January 10, 2013 07:23

Hi Mads,

User zaynah's has found the solution which was I think related to the problem setup as we were discussing in another thread. If you don't mind, I have a question regarding what you said above.

You mentioned relatively lower courant number/time step size required for explosion problems? Or do I understand it differently? I am working on explosions and my simulations sometimes result in very low courant numbers (lower upto 0.01 and time steps upto 1e-15s) when adjustTimeStep is enabled with maxCo typically around 0.2. The problem that I often face is the courant number calculated using the typical velocity, timestep and cell size, which is of order 1e-8s, does not always apply- infact sometimes the time step size required is 10 or higher times than calculated for stable calculations.

I am not sure my explanation is clear enough but any information would be helpful regarding the treatments required in such problems.

zaynah04 January 10, 2013 07:30

Hi Mads,
i will come back to you later with this..I am currently stuck somewhere else..:(

I have successfully iterated around 6 case and achieved convergence...

Suddenly for all the 6 cases i get this same error!!
can anyone tell me what is wrong ?


cannot find file

file: /home/zaynah/Desktop/system/controlDict at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

MadsR January 10, 2013 11:10


I am not sure I understand your question. I don't think explosions, per say, needs low Courant numbers, as it of course also depends on your mesh, but they sure needs low time-steps (relative to more "normal" simulations).
I would expect, being completely ignorant of explosion simulations, however, that you would run at a very low min-Courant number as I would expect that your cells are quite large in certain (most) areas because of the development of an explosion-plume (or what you call it) into the surroundings...I am just guessing here though.


Traib January 10, 2013 11:37

Thanks for your reply Mads. Yes, the cells are of quite varied sizes, larger at regions far from core combustion region. I just realized I was using max time step as the limiting parameter with low courant number calculated using smallest mesh size, instead of using an appropriate courant number to control the time step, which resulted in significantly decreased time step sizes in densely meshed areas where temperature also increase significantly. This strangely enough seems to be the cause of the error and with a limit on courant number time step sizes are adjusted to about the calculated values. I suppose I just had to try this different approach for stable results.

zaynah04 January 10, 2013 12:35

Dear Mads,

lets come back to the low courant number..;-)

My velocity is 0.0001m/s courant is 2.4 e-6.

i am simulating some simple case for comparison with other softwares.. I have to decide which software is best suited for my project.

I have not modify the time step.

It seems that you have tried to lower the time step much to achieve convergence?
i will be waiting for your analysis..

ps: for good convergence what must be display in terminal? i mean for me to know that the solution has converged??

All times are GMT -4. The time now is 20:26.