open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

I am currently trying to model the influence of row of blocks in a mountain stream. I encounter few difficulties among which this one :
when drawing a cross-section where stands the row of block, there is like a huge meniscus, that is to say water depth is highly decreasing approaching the block which seems to me really unrealistic.

I first defined the blocks as liable to flooding (change in bathymetry) then as unsinkable (as a contour/outline) in Matisse. The problem remains.

Any advices ?
Thank you very much for any help

Pauline


For the records, my other problems are :
- instability upstream far from the row
- high values of turbulence intensity (I=sqrt(K)/V) far from the row (about 20%).

Hello,

If you treat a block as a bump on the bottom. The theory says that in sub-critical flow this decreases the free surface above, and in supercritical flow there is also a bump in the free surface. If the water depth decreases too much it may trigger that the flow becomes supercritical above the bump, and then there will be a hydraulic jump. SO it could be that what you find is not so unrealistic. With islands it is the same behaviour, the free surface decreases between the islands.

WIth best regards,

Jean-Michel Hervouet

Hello,

I am currently trying to simulate influence of a row of blocks (diameter 40cm) in a 1%-slope 6m-wide flume.

I encounter a few issues that I doubt to be linked :

- Turbulence intensity (I=sqrt(K)/V) is very high (about 20%), even far away from the blocks (and by the way even without row of blocks). I used a k-epsilon model. I looked in bibliography any data to compare without success but it seems too high to me.

- When drawing a cross section profile, water I observed like a huge meniscus between the blocks, with water depth highly decreasing near the block. I seems wrong to me. I first defined the blocks as liable to flood (change in bathymetry) then unsinkable but the problem remains. I don't understand.

- Instability upstream far from the blocks row appears after a long time of simulation. At first, I did not see it, because I did not wait enough. I try many changes but it remains. This one is a very complicated issue. I don't think you can help just with my explanations but even if I doubt it, maybe it could explains the other issues.

Any piece of advice ?
Thank you very much for your help
Pauline

First I'm sorry I posted twice. Thank you very much for your quick answer.
Here is a picture of the cross section profile. It seems to me that the evolution between two islands is the opposite.

Hello,

Your results seem correct, assuming that flow goes from bottom to up in the upper picture: water level higher upstream on the block (kinetic energy changed into potential energy), water level lower immediately downstream the block, and between blocks level decreasing due to the narrowed passage (Venturi effect).

Regarding the k-epsilon model, you should perhaps look at the turbulence level at the entrance of the domain. It is hardcoded in Telemac subroutines (see kepscl.f in library telemac-2D) and it assumes some balance between friction and turbulence. Generally users have a domain which is too small to see the real k-epsilon model fully established, and they just mostly see their boundary conditions at the entrance of the model.

With best regards,

Jean-Michel Hervouet

Thank you for your answer. It helps a lot !
Would you have an idea of the length of domain to enable k-epsilon model to establish.

I tried to realise a simulation in a 500m-flume (slope :1%, width=6m, Ks=25, mesh=0.5m)to evaluate values of k and epsilon in order to know k and epsilon values I could put at the entrance of the domain. But values remains the same all along.

Is there an other way to evaluate the values at the entrance.

By the way, very good book, it helps a lot !
Thanks,

With best regards,
Pauline Prel

Hello,

Well, I refer to 3D simulations where you see the boundary layer slowly increasing from the entrance of a domain. In your case and in 2D, 100 m or maybe less should be OK. You can look at the test case of folder test.fr, called dragforce, which uses k-epsilon. Note that with k-epsilon you must have your VELOCITY DIFFUSIVITY = 1.E-6 (a common error consists of having a larger value trailing from previous computations with turbulence model = 1). Generally speaking, I do not think that k-epsilon model brings a lot of improvement in 2D, as it takes into account also dispersion, which is larger than turbulence sometimes. Purists will tell you that 2-dimensional turbulence does not exist or is a very specific phenomenon. I always give the advice of trying first a constant velocity diffusivity equal to 0.1, then when everything is OK in your computation, you can see if k-epsilon brings an improvement.

With best regards,

Jean-Michel Hervouet