open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,
I just compared the computed results of TELEMAC-2D with computed results of HYDRO_AS-2D and MIKE 21. When I look on the velocity distribution over a cross section in a trepezoidal cross section then the results of MIKE21 and HYDRO_AS-2d resemble but the results of TELEMAC-2D are different as shown in the attachment.





Furthermore, the free surface elevation on the sides is higher compared to the middle of the profile. I can't imagine that this is realistic!?

Does anybody have an idea why the velocity profile looks that different?

Cheers
Sarah

Hello,

Can you share your TELEMAC-2D simulations files with us, so we can have a look ?

Sébastien.

Sure, sorry i forgot them!

Cheers Sarah

Hello,

On the elevation on the sides, is it not just a linear interpolation between the last point with water and the first dry point that gives the impression that we have a slope ?

On the velocity profile, it is highly depending on the turbulence model used, so it is the thing to compare.

Regards,

JMH

Hi!

Apart from the remark on the choice of turbulence model used that can influence your velocity profile in the cross section, your downstream BC definition might also influence your velocity profile especially near the boundary. You prescribe Q = -3900 m3/s with a rather constant velocity profile which doesn’t seem to be physical, unless you want to reproduce a real case.
Why did you not use a prescribed elevation instead?

I also note that you have a pretty high roughness coefficient (100)…

Regards,
PL

Hi,
But is it really a question of the turbulence model, because in this area of the model there is a nearly undistrubed flow without large turbulences. It is actually a one-dimensional flow.

The point of the velocity profile seems reasonable to me. But the cross section is about one kilometer away from the outflow boundary. Can this affect the velocity distribution so far away from it?
How would you define the velocity profile?

The bed friction is that high because it is a concrete canal. In the other simulation software the same bed friction was used.

Cheers
Sarah

Hi,

The choice and set-up of a turbulence model will influence your computation even if what you model is suitable with a 1D flow. You see for instance in your graphs that you do have a non constant velocity profile across your section.

Try the following:
- Velocity diffusivity = 0,1 m2/s and not 1,0 with constant viscosity turbulence model
- TURBULENCE MODEL = 4 (smagorinsky) or 3 (k-epsilon) with Velocity diffusivity = 1.E-6 m2/s.
You should obtain something that is more close to what the two other models give.

What were your turbulence settings with MIKE21? Constant viscosity or Smagoringsky?

On boundary conditions, if you choose 5 4 4 (prescribed elevation and free velocities) at the downstream end, the velocity components at the boundary will be in accordance with your flow pattern in the vicinity of the boundary, which is usually what we want to have.
For upstream, you can maybe try VELOCITY PROFILE = 4 which will give velocity components proportional to sqrt(H), which tends to a relatively more "natural" profile, ie similar to what the program computes in the middle of the reach.

Good luck!
PL

Hello pilou,
thank you for your answer. When I change the ruurbulence parameter the results are comparable to the other models. But now there is a oscillation in the peak of the velocity profile (see picture). Do you have an idea what is the reason for that?



Another question was coming up when I tried to adjust the simulation parameters to them of the other models. When I use the finite volume equations with a variable time step then the prescribed discharges are not complied. Then the inflow is about 4340 m³/s and the outflow -4180 m³/s? Do i have to consider anything else when using the finite volume method??

Cheers Sarah

Hi,

On the oscillations: are you sure to obtain a steady state prior to extracting your profiles? I say that because sometimes the default values could be a bit too large to actually identify the moment when the steady state is reached, especially when you look at small evolutions on small time steps. Try to launch the computation over a long period and compare the results in the end.

Oscillations may also be due to the choice of turbulence model. I think other persons might have better advices but as far as I know it wouldn't be strange to obtain such a profile with k-epsilon for example...

On finite volume method, here also other persons might have better advices but did you add DESIRED COURANT NUMBER = 0,8? Running finite volumes with higher CFL number tends to unstable computations so it could be a possible explanation...
Another possible cause would be to use 4 5 5 (prescribed discharge -3900 m3/s) as downstream BC. I think this is an ill-posed problem as you don't prescribe any water level at any boundary! It maybe gives not so stupid results with finite elements but does not work with finite volumes. Be careful with that...

Good luck!
PL