CFD Online Discussion Forums - Courant number in OpenFOAM

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM (https://www.cfd-online.com/Forums/openfoam/)

- - Courant number in OpenFOAM (https://www.cfd-online.com/Forums/openfoam/180202-courant-number-openfoam.html)

Courant number in OpenFOAM

When do i need the folowing equation?

https://openfoamwiki.net/images/math...d5a50a961b.png

And what does it mean?

is there Delta V the cell volume and Delta S a area from the cell surface? What means the f in sum_f.

Could somebody explain it with a cell with the size a*b*c

found it on:

https://openfoamwiki.net/index.php/Co

and also in CourantNo.C

Code:



tmp<volScalarField::Internal> Coi

Code:

                

(                                   

  byRho

  (

     (0.5*mesh_.time().deltaT())

     *fvc::surfaceSum(mag(phi))()()                                          

     /mesh_.V()

   )                               

);

The Courant number provides a stability criterion, which is especially important if you use an explicit time scheme. If

, you may expect your simulation to diverge. See:
https://en.wikipedia.org/wiki/Couran...Lewy_condition
Intuitively, it says that within a given timestep $\Delta t$ , fluid may flow a distance $U\Delta t$ of one cell $\Delta x$ at most (if

). In practice, we limit the Courant number to be smaller than 0.1~0.5.

In your equation
$\Delta x = \Delta V / \Delta S$ ,
where $\Delta S$ is the surface area of a face. Plugging in your

, you will find that

(for example).
This expression should be evaluated for each face

, because (again, see the link above) in more dimensions you should sum the contributions of each dimension. The factor 0.5 is presumably there to prevent double-counting opposite faces (west and east), as they belong to the same direction.

When do you need it? You don't.
In controlDict, set

Code:

adjustTimeStep  yes;

maxCo           0.25;

and OpenFoam will automatically limit $\Delta t$ as to have a Courant number below "maxCo".

Well this is everything i need t know. Thank you.

Automatic Control of Courant Number

Quote:

Originally Posted by floquation (Post 626157)

When do you need it? You don't.
In controlDict, set

Code:

adjustTimeStep  yes;

maxCo           0.25;

and OpenFoam will automatically limit $\Delta t$ as to have a Courant number below "maxCo".

At what point in the Control Dictionary does this go. I tried to use it with icoFoam and still had severe convergence problems.

Thanks in advance.

The factor of 0.5 is just because we summed over the magnitude of the phi, since the phi_in hast to be equal to phi_out. Is that correct?

Quote:

Originally Posted by superkelle (Post 776086)

The factor of 0.5 is just because we summed over the magnitude of the phi, since the phi_in hast to be equal to phi_out. Is that correct?

yes Sir, thats correct.

Quote:

Originally Posted by HappyS5 (Post 697831)

At what point in the Control Dictionary does this go. I tried to use it with icoFoam and still had severe convergence problems.

Thanks in advance.

Hello,
icoFoam has not this feautre implemented, if you want "icoFoam with adjustable time" you should run pimpleFoam in ico foam setting and pimple has adjustable time build in.
best regards