[fimbull]

When do i need the folowing equation?





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

tmp<volScalarField::Internal> Coi

                
(                                   
  byRho
  (
     (0.5*mesh_.time().deltaT())
     *fvc::surfaceSum(mag(phi))()()                                          
     /mesh_.V()
   )                               
);

[floquation]

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 , fluid may flow a distance of one cell at most (if ). In practice, we limit the Courant number to be smaller than 0.1~0.5.

In your equation
,
where 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

adjustTimeStep  yes;
maxCo           0.25;

and OpenFoam will automatically limit as to have a Courant number below "maxCo".

[fimbull]

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

[HappyS5]

Originally Posted by floquation

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

adjustTimeStep  yes;
maxCo           0.25;

and OpenFoam will automatically limit 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.

[superkelle]

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?

[geth03]

Originally Posted by superkelle

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.

[otaolafr]

Originally Posted by HappyS5

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

[wolf.bkh]

Originally Posted by floquation

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 , fluid may flow a distance of one cell at most (if ). In practice, we limit the Courant number to be smaller than 0.1~0.5.

In your equation
,
where 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

adjustTimeStep  yes;
maxCo           0.25;

and OpenFoam will automatically limit as to have a Courant number below "maxCo".

Hi,

I am a beginner on OpenFOAM an I am working on gas Leakage and Dispersion into a room. As the source of leakage can be very small (for example a source of 10 mm of diametrer in a room of 10 m3)I am obliged to apply a high refinement around the source . So I would like to know if it is possible to set different Co_max number and how ?

Best Regards,

Wilfried B.

[Tobermory]

It depends.

Do you need to model the transient behaviour in a time accurate fashion? If so, then Co must be less than one, and a max of 0.5 is often sufficient to prevent the solution blowing up.

If you are only interested in the final, steady state condition, then you can use the PIMPLE algorithm and sometimes get away with a much higher Courant number ... or just use a steady state solver instead.

[wolf.bkh]

Originally Posted by Tobermory

It depends.

Do you need to model the transient behaviour in a time accurate fashion? If so, then Co must be less than one, and a max of 0.5 is often sufficient to prevent the solution blowing up.

If you are only interested in the final, steady state condition, then you can use the PIMPLE algorithm and sometimes get away with a much higher Courant number ... or just use a steady state solver instead.

Thanks for the feedback. At the moment I'm working on a test case, so I'm much more interested in the final result, before making my parameters more complex.

Best Regards,