open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

I'm working on the erosion phenomena of a gravel beach. I've already simulated the interaction between the waves and the current by an internal coupling between Tomawac and Telemac2d.
Now, I would like to link the action of the waves and the wave driven current (no tidal effect) to the sediment transport. So I've planned to use Sisyphe. I have some questions in order to be sure of the way to do it, and the limitations of the method.
1) For what I've understood in the current version of Sisyphe I cannot internally couple Telemac2D/Tomawac/Sisyphe ?
2) What could be the most precise coupling process to take in account for unsteady waves and current ? I have found some answers in :sisyphe_user_manual_v6p0_2, p39; but I don't understand how I can " store all the wave and hydrodynamic relevant variables on the same input ‘HYDRODYNAMIC FILE’ " ?

Regards,

Rémi.

Dear Rémi,
the internal coupling Telemac-Tomawac-Sisyphe is being tested. It will be incorporated in the new release of the Telemac-Mascaret system (mid-year). This will be a "clean" way to incorporate the three processes (also with the possibility of choose the coupling period for each code).

Kind regards,

Pablo

Hello,

Thank's for your answer Pablo,

I've started to use a chained method to link TOMAWAC-TELEMAC2D and SISYPHE (because I would need to have results now, I cannot wait for the new version of TELEMAC...).
It runned quite well but I've got some weird results on the boundraies (see picture attached)... Especially when you check the "evolution" variable.
Do you know where it could come from ? I must have done something wrong but I cannot find what it is.

I've attached my boundary condition file (geoCourantSEb.cli) and my sisyphe case file (Sisyphe.cas).

Thank you for your time,

Regards,
Rémi

Hello Rémi,
I took a fast look to your 'cli' file. I noted you have a boundary 5 4 4 between the nodes 4055 and 53900.
Then, you have a boundary 5 5 5 imposed only on 2 nodes (43504 and 43405). Is it OK for your problem/domain?

Below some hints:
- take a look to the values of shear stress (shear velocity US) of your problem
- in your boundary 5 4 4 you are 'fixing' evolution of the bathymetry by imposing the flag '5'. Run a test by putting '4'.

Let me know,

cheers

pablo

Hello Pablo,

Thank you for your quick answer !

About my boundary file I have 5 5 5 imposed on 2 nodes because I added a stream to my model. To run the Hydrodynamics models (Tomawac and Telemac) I had to set the boundary with prescribed discharge and height (5 5 5).

I tried to change the tracer boundary condition as you suggested from 5 to 4, but the simulation is not running anymore. The error is : "Negative depth prescribed on boundary, check your specific subroutine BORD3D"
Initially, I've set the tracer boundary condition at 5 because I've read it on the validation files of Sisyphe : "07_littoral_Dunkerque"...
But I agree with you it should be more logical to have a free (4) evolution of the bottom at the boundary.

I'm trying to change some parameters but I really don't know why I have this error of negative depth ...

Cheers,
Rémi

Hello,

I really don't know why I have these values of bottom evolution on the boundary.. I read the "solid_discharge_sisyphe_2012-10-05.pdf".If I set LIEBOR=5 (KENT) and LIQBOR=4 (KSORT) for boundaries I can prescribed variation of elevation. By setting EBOR to 0 it should solve my problem...
But I don't get why nothing changed.

I tried a lot of boundary conditions changes, and with LIEBOR=4 I always have the "negative depth problem".

I'm completly stuck here, could someone help me ?

Thank you,

Regards
Rémi

Hello,

Actually the message comes from subroutine positive_depths (library bief). It should probably say BORD3D OR BORD. What I suspect is that you have a prescribed elevation on a boundary, then the depth is (this elevation) - (the bottom). If a deposition occurs and the bottom goes higher than the prescribed elevation, it would give a negative depth and we obviously need to put a control there, prescribing a depth=0 instead. However in the standard subroutine bord, HBOR is always given in the form MAX(0.D0,...) so it must be positive, maybe you should check your own subroutine bord.f if any.

With best regards,

Jean-Michel Hervouet

Hello again,

Better idea:

In fact, positive_depths is also called for solving the Exner equation (by bedload_solvs_fe), so it could be that the prescribed sediment thickness is negative, due to some misunderstanding in the boundary conditions. This would be then a problem. As all is based on the fact that positive_depths is designed to keep a positive thickness, it stops if imposed a negative thickness. I'll change the message so that it does not mention only BORD3D, which is certainly misleading. No we have to understand why this prescribed thickness is negative...

JMH

Hello M. Hervouet,

I think you're right, it should come from the fact that I have this big deposition on the boundary (see previous post with the picture). Because of this phenomenon, I get a bottom which is going higher than the prescribed elevation. So, I'm not sure but I think that my problem of negative depth is caused by the high values of bottom evolution on the boundary...
What do you think ?

I'm also trying to study what you've suggested about the prescribed sediment thickness..

Thank you for your time,

Regards,
Rémi

Hello,

Yes, you must have an imposed evolution that removes all the available sediment. A possible bypass of the problem would be to add a line in subroutine bedload_solvs_fe.f after line 177. This line is:

T8%R(K)=AVA(N)*EBOR%R(K)*CSF_SABLE+HZN%R(N)

you could add after :

T8%R(K)=MAX(T8%R(K),0.D0)

however it would be better to cure the problem at the origin, where an EBOR is prescribed that will remove all the available sediment.

This does not explain why you have large depositions. Obviously after some time you have tidal flats, are all the right options of tidal flats set both in Telemac-2D and Sisyphe ?

Regards,

JMH