open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello!

I'm a new user of Telemac 2D. I'm running v6p3 for a 30 km river model with 4 boundaries(BC1 = prescribed H and BC2,3,4 = prescribed Q).
I impose constant Q and H in order to reach an "initial" steady state :
SL(1) = 0.5 mNGF ; Q(2)=40 m3/s ; Q(3)=2 ; Q(4)=2.

My problem is that flux balance is not conserved along the model, flowrates downstream are higher than imposed inflows.
An example of flux balance given by Telemac is attached. It's for the last time step of a 2 day simulation.

I inspected flows at some cross sections of the riverbed using BlueKenue and it appears that in some parts, flowrates increases along the riverbed.
--> Attached plot n°1 shows Q(t) for successive X-sections along a 3km tributary riverbed ("Peyne01" the dowstream one and "Peyne07" the upstream one)
--> Attached plot n°2 shows Q(t) upstream and downstream weir in main riverbed
I checked Froude number results at these problematic zones and it shows very hight values at some nodes (around 10000 for somes...).
At the same nodes, velocities and water-depths/flows have instabilities.

I thought problems came from high-bank slopes + poor node density at problematic zones, so I tried to densify my mesh (x 5) at concerned areas. At the result, flow increases, froude numbers and water depth instabilities are a bit reduced but the problem remains.

I also applied advice given by users on the forum for the CAS file :
COMPATIBILITE DU GRADIENT DE SURFACE LIBRE = 0
COEFFICIENT DE DIFFUSION DES VITESSES = 1
Those parameter modifications improved results, reducing differences in flux balance, but the increasing flows remains... (Flux balance attached is the "best" I coud reach).

I don't really know if my problem is due to a bad mesh density or the bathymetry profile or some bad choices for parameters.

Does anyone have an idea for how to solve this?
Thank you very much!

(My CAS file is attached)

Hi Locness,

Did you already try COMPATIBILITE DU GRADIENT DE SURFACE LIBRE = 0.9?
Could you please attach your simulation (geometry, boundary and steering) files? That would be helpful.

Cheers,
José Andrés.

Hi Locness,

your steering file looks ok.
However, I would turn off CLIPPING DE H and turn on CORRECTION DE CONTINUITE

Hope this helps,
Clemens

Hi Locness,

two days are maybe not long enough to reach a steady-state for a 30 km river model. This also depends strongly on your initial condition.

It can help to compare the solution for last and the second last timestep. I usually plot the differences between h,u and v. This helps also to identify problems with boundary conditions.

Cheers,

Leo

Hi Leo, thanks for your reply!


When I look water depth, free surface and Q plots, it looks like a "steady state" was reached? Moreover I first used to compute 3 days simulations reaching similar state. So I thought 2 days was long enough...

I don't really know how to create an initial condition for my riverbed water depth.
As I said in my previous repply, I use water-depth result from previous computation + adding water-depth values in some riverbed parts using bluekenue map-object tool. But initial condition doesn't have velocity values and initial free surface isn't "physical".
Maybe it impacts in wrong ways the next calculations steps?


Regards,

Loïc

Hi José Andrés and Clemens, thank for your replies!!

Yes I initially used "COMPATIBILITE DU GRADIENT DE SURFACE LIBRE = 0.9" but using 0 as value, as advised in other topics, iproved results making outflow values closer to inflows, so I kept using 0.

I also tried an other configuration in my steering file using :

CORRECTION DE CONTINUITE : OUI
EQUATIONS : 'SAINT-VENANT EF'
IMPLICITATION POUR LA HAUTEUR : 1
IMPLICITATION POUR LA VITESSE : 1
TRAITEMENT DES HAUTEURS NEGATIVES : 2
PROFONDEUR LIMITE POUR PROCEDURE DE RESSUYAGE : 0.01

Results are better in terms of stability and flows!

Moreover I made an other simulation reducing time steps from 2 to 1 sec. It also improved results, reducing flows difference between upstream and downstream!

Finally I identified and fixed some nodes with more than 8 neighbors in my mesh. Results of simulation seems better in terms of velocity stability!

I'll try to combine all this and make new simulation...!

___________________________________________________________________
However, here are my simulation files :

Geometry file : 'GEO_HerAv_Ks4'
BC file : 'BC_ModConc_Ks4'
Steering file : 'CAS_Ks4'
Previous computation file : 'RES_avSS_Ks4'

The previous computation file was created in order to start simulation with water in the riverbed.
BOTTOM mesh is the same as in the geo-file.
WATER DEPTH mesh was created in 2 steps.
--> First a simulation was made, only imposing constant free surface = 0.5 m (no inflows), in order to fill sea and downsstream riverbed parts.
--> Then waterdepth mesh was modified with bluekenue, mapping water depth in dry riverbed zones (upstream parts).


Best regards,
Loïc

Here are the 2 attached files missing

Well, I can't put GEO and Previous computation files here (maybe too heavy?).
If needed I'll send them by e-mail

Loïc