open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,
In reference to the simulation result posted at
www.opentelemac.org/index.php/kunena/16-...lation?start=10#7747

I have observed that the flux across the intake boundary varies with respect to the free surface variation in the channel, or the tidal value imposed at the outer boundaries. The variation is about 1 m3/s. But the intake discharge is given at a constant rate of 5.5556 m3/s at the boundary.
Also while the simulation is running it can be observed that the flux listing across intake is varying.

Is there any explanation for this varying flux across the intake boundary?

Regards,
Gourih

Hello,

If your plot is the flux given by a cross section, there may be a difference (the more so if the cross section is not exactly at the intake). The flux intake is added in the continuity equation, so it is the real amount of water entered in the domain, if you do a mass balance. The flux given by a cross section depends on the local velocities, the difference has something to see with the finite element approximation. A more striking difference happens on solid boundaries. If you discretise badly near a solid boundary, you may see velocities going across the boundary, however the quantity of water going through the solid boundary is zero because the flux across the solid boundary in the continuity equation is given as zero, whatever the velocities observed. We can only hope that the two values will converge when space and time steps tend to 0.

Regards,

Jean-Michel Hervouet

Hi Jean-Michel Hervouet,

Yes the flux is given by a cross section along the elements just next to the intake channel boundaries.

I shall try to get the flux across the intake listed in a file during the simulation run to check the actual values.

The explanation was really helpful to me.

Thanks and Best Regards,
Gourish

Hi,
While analyzing the intake problem of varying discharge, I had put two intake discharge boundaries, in the simulation. Both the intake discharge have the same rate .i.e -5.5556 m3/s.

The flux at first boundary shows variation as I have mentioned earlier, and the second shows the flux value constant as per the discharge value provided.
This is evident from flux listing in the simulation run.

Even when I put more than 2 discharge boundaries the first boundary always shows varying flux, and the other discharge boundaries show constant flux.



Is it an expected behavior, or do I have to change the way as how the discharge forcing are given.
I have attached the case, boundary file and the liquid boundary file.
The geometry file and fortran file is same as per the link
www.opentelemac.org/media/kunena/attachments/2535/rilEx5m3.zip

Regards,
Gourish

Hello,

In your steering file I would expect the line :

PRESCRIBED FLOWRATES : 0.;0.

that triggers the call to function Q (otherwise the values of velocities in the boundary conditions file are taken). So I am actually surprised that it works at least for one boundary (probably because I have added recently an extra test to see if the liquid boundaries file exists, and decide to use it in this case).

The keyword PRESCRIBED ELEVATIONS : 0.

also gives a value 0. only for the first boundary, so probably 0.;0.;0. is necessary to reach the third boundary and trigger a call to function SL.

But in fact your problem comes from the keyword :

OPTION FOR LIQUID BOUNDARIES : 2

that put Thompson on your first boundary, it should be :

OPTION FOR LIQUID BOUNDARIES : 1;1;2

Another thing I noticed is that the tracers in the boundary conditions file are declared like on a solid boundary (2) instead of 5 for liquid and prrscribed.

This will probably help have the correct behaviour, have a good week-end,

Jean-Michel Hervouet

Hi Jean-Michel Hervouet,

I made the changes in the case file as you have mentioned, and now the simulation is working properly. I am able to observe the correct flux at the boundaries as mentioned in the boundary condition.

Thanks and Best Regards,
Gourish