open TELEMAC-MASCARET The mathematically superior suite of solvers

Dear all,

I'm doing a numerical model of a river in Switzerland exiting in Lake Geneva for my master thesis. The goal of my project is to evaluate morphological change of delta with river floods, high wave events and high winds events.
I have two liquid boundaries. The inlet boundary (BC number 2) (prescribed Q) is located at 386 amsl and the outlet boundary (BC number 1) (prescribed H) is located at 372.10 amsl. For the BC 2, I have a liquid boundary file allowing to slowly grow the discharge (Q goes from 0 to 40 m3/s in 4500s) and I give to my model also the surface elevation variation during the same time span. My time step is set to 0.5s and the solver accuracy to 10^-3 and I set the INITIAL CONDITION AS "CONSTANT ELEVATION". I fixed an initial elevation of 385.8 amsl filling my whole domain with water and it runs without entering supercritical entry with free depth but took some time to converge to only river flow.
Thus, since I need to couple sisyphe-tomawac-telemac I would like to reduce the computation cost so I try to have as initial condition an initial elevation of 372.10 asml (the level of Lake Geneva). However I entered in supercritical flow which is logical due to the elevation difference. From what I have understood from the previous forum, I need to "dig a large pound" in my bathymetry close to the boundary could you tell me if it's the optimal method for my case to allow water flowing through the river or if there is a best way to fix the problem in my case ? If it is, how to perform a such hole ? Should I have to do as in baxter-tutorial for the levee modification in Blue Kenue?

NB : you will find attached to this mail the necessary files if needed.

Best regards,
Alexandre

Dear Alexandre,

Is it correct that you are looking for a better / smoother initial hydrodynamics for your coupled simulation run?
In that case you can use the water depth and velocities from a PREVIOUS COMPUATION FILE done before only running telemac2d.
Best regards,
Rebekka

Hello,

thank you for your reply, it is this kind of effect that I try to have but actually, I tried with hotstart but I have also free velocity problem at my inlet boundary, that is why I tried to fill my domain with water (but it creates too much erosion) or to dig a hole in the bathymetry at my inlet boundary condition but it acts as a huge trap for sediments such that the bed is only aggrading at my solid discharge inlet boundary leading to free velocity ...

Regarding to hotstart I tried but obtain also free velocity problem at inlet boundary condition but maybe I'm doing something wrong.

I attached my simulation files below and add a screenshot of the the bed evolution where we clearly see the effect of the hole in my bathymetry at the boundary.

Best regards,
Alexandre

Hi all,

Thanks to Rebekka I explored hotstarts and obtained better results this way for sediment discharge with no more sediment trap due to the "pool" I was digging (so many thanks to Rebekka).
However, I still have inconsistencies regarding to bed evolution since lots of deposition occurs at my BCs, in 2 days I have an order of magnitude of 7m of deposition near one of my boundary nodes and 2m of erosion in a BC point next to it. Actually, it seems that sisyphe did not distribute sediment along all the BC nodes. I mean that the first mentionned node received most of the solid discharge. However, it's not the deepest node of the boundary but nor the highest regarding to elevation. Do you have any suggestion to go beyond this problem ?

In the here above figure, you have the bed evolution (surface) and the solid discharge (isoline).



Best regards,
Alexandre

Dear all,

The result is almost here, by resizing the inlet solid BC to the BC points close roughly corresponding to the river bed, I obtained less sediment accumulation ~ 1.9m instead of 7m. I however have erosion of 2.9m at BC so I think I will try to fix a non-erodable bed below 2m to avoid too much erosion at BC point, is this a solution to your opinion or have I to work on my mesh (I'm not fully satisfied by the mesh at outlet BC) and to look at numerical parameters (ie problem in my BC/initial conditions ) ?





I'm however a bit surprised that after 2 days of simulation with bedload inputs, I only have small bed evolution at river outlet in Lake Geneva.





Do you think I have to extend my simulation time ? Or doing a hotstart with this result file ?

I also have to couple TELEMAC-2D and SIYPHE with TOMAWAC, do you have any advice/hint to decrease computation time ?

Below, my mesh at inlet BC :



Below, my mesh at outlet BC :




Best regards,
Alexandre

Dear Alexandre,

I am glad that you could manage your simulation.

Concerning the grid: We always care a lot about the open boundary mesh because this avoids numerical problems which comparably small costs. The best mesh at the boundaries are equally spaced 60° triangles (like a sawtooth). Non-erodable bed at the inlet is additionally a good option.

As there is nearly never a (quasi) steady state in morphodynamics I would guess that 2 days are not long enough but of course I can not say that for sure.
You could use the morphological factor (carefully) to speed up the telemac-sisyphe simulation. It is hard to say up to which factor it is safe, so you should always do a check comparing a simulation period with and without the morphological factor. For waterways we use morphological factors between 4 and 10. If you use a hydrograph you need to compress it with the morphological factor.
Unfortunately I am not familiar with tomawac so I don't know how to speed up there or if using a morphological factor (on time scale) can be used together with tomawac.

Best regards,
Rebekka

Hello all,

Thank you very much for your answers.

According to what you say Rebekka I will try to obtain equilateral triangle for the outlet of the river. I will also try the morphological factor it seems to be a good way to work and the non-reodible bed, thank you again for your advice. Is-it possible to define the non-erodible bed with a polygon through BK or should-I use Fortran coding ? Have you got an exemple fortran file where you define the zone of non-erodible bed that you can share with me/us ?

Mafknaapen, I'm unfortunately working on a wave-dominated delta so I will need wave driven currents since the wind and the associated waves are the main source of currents in Lake Geneva... but it will be a good challenge to play with timesteps. For waves generation, a good work was previously done by swisslakes.net/ to model wind-wave generation so I will use these previously compute results as boundary condition.

Best regards,
Alexandre

The 3-way coupling with TOMAWAC will always be relatively slow, but there are ways to
minimise the computation time:

1. avoid using dissipation by a strong current
2. if you don't need it, turn of wave driven currents in TELEMAC
3. play around with the time step of TOMAWAC, as it is not a linear relationship between time step and computation time. Due to the matter of characteristics in a changing flow a very large time step will sometimes slow the computations down instead of speeding them up.
4. use TEL2TOM with a coarser mesh for the wave computations

But it is very likely that you just need to be patient.

Good luck!

Dear Alexandre,

I am not using Blue Kenue so I don't know how to define a non-erodable bottom there.
As your river is north-south directed at the inlet it would be easy to do it in fortran according to a specific y-coordinate and according to the friction coefficient in the subroutine noerod.f. See a sample coding below.

Best regards,
Rebekka

USE DECLARATIONS_SISYPHE, ONLY : CHESTR
IMPLICIT NONE

INTEGER I
!
!

---

! RIGID BEDS POSITION
!

---

!
! DEFAULT VALUE: ZR=ZF-100.D0
!
CALL OV('X=Y+C ',ZR,ZF,ZF,-100.D0,NPOIN)
!

DO I=1,NPOIN
! non-erodable bottom for y> 1000 and a roughness coefficient which is between 0.059 and 0.061 (assuming that the river has 0.06 m roughness coefficient)
IF(Y(I).LT.1000.D0. AND.
& (CHESTR%R(I).GT.0.059.AND.CHESTR%R(I).LT.0.061)) THEN
! non-erodable bottom = bottom
ZR(I) = ZF(I)
! non-erodable bottom = bottom - 0.1 m
! ZR(I) = ZF(I) - 0.1
ENDIF
END DO

Hi all,

Thank you Rebekka for your piece of code, I adapted it and it works well. I attached the fortran file with few comments if someone needs help to adapt it :


Just to be sure, regarding to morphological factor. If I set it to 2, are we agree that, since I have time-varying BC in sisyphe and telemac, I need to compress (divide by 2 the time) only in telemac liquid boundary condition file to maintain the consistency between liquid and solid discharge ?


Best regards,
Alexandre