open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

I am trying to make a telemac2d model for a parking which is flooded. I have a river at the upstream of this parking and the water is stocked in a kind of dip (big hole) before to overflow on the parking. I already post about BC of this model lasr week and following your advice i made as follow :

- I create a deep zone on my upstream BC.
- I fill this deep zone using BC(566)
- I used the result file as PREVIOUS COMPUTATION FILE
- Then I use a BC(455) by giving an hydrograph in the LIQUID BOUNDARIES FILE

So it's working during the first 490 iterations but at the 490th iteration the program stop saying :

DEBIMP : PROBLEME SUR LA FRONTIERE 2
DONNER UN PROFIL DE VITESSES
DANS LE FICHIER DES CONDITIONS AUX LIMITES
OU VERIFIER LES HAUTEURS D'EAU

So it seems that it become a supercritical flow at this time. But i don't understand why because the deep zone is still full and the flow at the upstream BC 2 : Q(2) = 2.8 while at the beginning of the simulation Q(2) = 0.1 and at step 230 Q(2) = 4.8.

So we have :
Step O Q(2) = 0.1 it work
Step 230 Q(2) = 4.8 it work
Step 490 Q(2) = 2.8 don't work

Moreover, during the first 480 iterations the flow have already overflow on the parking and runoff on its surface.

To resolve this problem i tried to use only a BC(555) giving discharge and depth in the LIQUID BOUNDARIES FILE. But the amount of water through the BC don't respect my prescibed Q (even with h that seems reasonable)
Q(2) = 2.8999999999999999
FLUX FRONTIERE 2 : 4.2222222

I though that telemac will adapt the velocity with prescribed H and Q to respect the prescibed Q.

Last information. I have no initial conditions on the parking (the parking is completely dry) but as i said before, during the 490 first step computation, the water spread to the parking

I join my result file in case of it can help.




Thank you for an help



Best regards

JP

Hello,

Yes, I have already seen this situation in a real application, conditions 4 5 5 (free depth and prescribed discharge) and if the flow becomes supercritical (so with larger discharge, exactly what you do), the problem is again not well posed, the free depth tends to 0 and it crashes. So you can either try an even deeper upstream zone or do a restart when the flow becomes supercritical again, but probably a deeper upstream zone would be simpler.

The problem Q(2) = 2.8999999999999999 and FLUX FRONTIERE 2 : 4.2222222
is probably because you have set CONTINUITY CORRECTION = YES. When you prescribe the depth, the continuity equation is no longer solved at the entrance, and the program considers that the FLUX FRONTIERE is the one that solves the continuity equation, not the one due to the computed velocities. You can check this by setting CONTINUITY CORRECTION = NO (the counterpart is that the mass conservation checking will be bad).

Regards,

Jean-Michel Hervouet

Hello,

Finally I made a deeper zone at the upstream zone... and i still have the problem (DEBIMP : PROBLEME SUR LA FRONTIERE 2...). So I looked for another solution : I pass the donstream boundary from (444) to (544) and it's work. It looks very strange because I am sure that the boubdary 2 is the Upstream One and the boundary 1 is the Downstream one.

Thanks for your help and for your quick answer to each post

Regards

JP

Hello,

As a matter of fact, your downstream boundary also has the same kind of problem, 4 4 4 is all free, and when the flow is fluvial it influences the upstream part (but what kind of depth could we impose here downstream ?). Stopping every time that a boundary changes its regime is probably the safer solution, though cumbersome. Another possibility (not yet tested in such case) would be to use Thompson boundary conditions, e.g. at the entrance impose both depth and velocity (to have about the correct discharge), and when the flow becomes fluvial the Thompson conditions would discard part of the upstream information. Anyway all such boundaries are artificial, this is why it is better to have a larger domain with boundaries that have a clear physical boundary condition (when it is possible..).

Regards,

JMH

Hello,

I will try withthe Thompson boudary condition and i will tell you if it's work better.
Even if I stop every time that a boundary changes its regime I still need to know the free surface at the Upstream and Downstream even if it's not during the entire computation time, so it's easier to define the free surface for the entire computation time.

I think I have not so bad results so thanks for your help.


Regards

JP