open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

I'm modelling a flume (30 m long, 6 m width, slope 1%, Ks = 25) with a row of small blocks at 19 m.
Instabilities in velocities and water depth appears in entrance of the model over a time step (see picture). The conditions in a entrance is flow fixed (4.7 m3/s for example), water depth is free, velocities are imposed.

I tried many things (reducing time steps, reducing mesh size, constant turbulence or k-epsilon model, defining a velocity profile in entrance, fixing water depth and velocities, Thompson which seems a little better maybe...) but I can not find where does these instabilities come from !

Would have any idea ? Any tests I could try to find out the problem ?
Thank you
Sincerely,

Pauline Prel

I had a picture if it works :

Hello,

The instabilities are the inf-sup oscillations that may occur if depth and velocity are discretized in the same way. This is theory. To overcome this there are several ways, the best one being to use the key-word :

COMPATIBILITY OF FREE SURFACE GRADIENT : 0.9

for example. The default value is 1. and you can go down to 0. if necessary.

Another way (less used now) is to use a quasi bubble element :

DISCRETISATIONS IN SPACE : 12;11

but this is much more time consuming.

I hope this helps,

Jean-Michel Hervouet

Thanks a lot ! It works.

I had to go down to 0.6 for "COMPATIBILITY OF FREE SURFACE GRADIENT" when I use a k-epsilon model.

It seems that it is due to the fact that I (have to) use a very very tiny time step (0.005 s) because of the blocks (where mesh is also tiny - 1cm) but at the entrance mesh is large (50 cm).

Again, thank you, I worked on this issue for 3 weeks !

Best regards,

Pauline Prel

Hello,

Unless your model is a small physical model at some scale, it is certainly not useful to have a mesh size of 1 cm. Unstabilities are more likely to appear at small Courant numbers. You can see for example the test case wesel in the folder test.gb (provided by BAW) with a number of groynes in a river. They are very refined, but maybe only with mesh size of 10 cm. This case works with a large time step and very high Courant numbers. The number of iterations of the solver is a good hint to know whether you can have a larger time step. Up to let's say 50 iterations it is OK.

With best regards,

Jean-Michel Hervouet