open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello everyone,

I am using telemac3d to simulate a vertical slot fishway. There is a lot of turbulence and I have tried k-e model, smago, and constant viscosity coeff. None of those gave me the correct turbulence.
This topic is following my previous one about the choice of a turbulence model.

Because of the huge geometry, I can only model one part of the problem. There is supposed to be a lot of turbulence in the entrance so I have to change the boundary condition of the k-e model.
I succeed to change the values of KMIN and EMIN in the SUBROUTINE CSTKEP, so the turbulence begins with high value (e-3). The results seem to be better but even the part with low velocity values have huge EMIN and KMIN (wich is logic).

I would like to continue the modeling (using the file .res) but I also want to change the KMIN and EMIN back to their previous values (e-10) to lower the turbulence in the dead zone. How can I do it?

Does a subroutine in which we can put the KMIN and EMIN back after a certain time laps exist?

Is there another way to put an initial condition for K and E ?

Thank you for reading

best regards,
Jean-Christophe De Greef

Hello,

KMIN and EMIN should remain small and are used just to prevent K and epsilon to become negative, this should be uncoupled from initial or boundary conditions. You can put at the entrance a turbulence that corresponds to turbulent energy being a percentage of the total kinetic energy (this is hardcoded in kepcl3, see the parts of code that are commented out, proposed as an alternative to EBORL=EMIN and KBORL=KMIN).
I would suggest that at least you use hardcoded values at boundary conditions and/or initial conditions, 1.D-3 if you want, but not through ELIN and KMIN, letting EMIN and KMIN at their smaller values. I do not believe too much in the effect in initial conditions (they will go away with the flow) but more in boundary conditions.
Think also that NUT=CMU*K**2/E, so that EMIN=KMIN=1.D-3 gives only NUT=9.D-5, it is not so high at the entrance...

With best regards,

Jean-Michel Hervouet

Thank you for your answer.
I knew it was not the right way to do. We only want I change the boundary condition and I put the formula that was in comment.
I don't understand the formula in comment for the "wall" part. How can a turbulence begin on the wall ? This part is just curiosity, I guess I don't have to change it.

Thank you for help, I begin to see clear in the code.

Hello,

The turbulence at the wall, according to the theory, is taken after the viscous layer, in the logarithmic zone, it is consistent with the fact that the velocity is not 0 at the wall, for the same reason. Generally as the mesh size is much larger than the viscous zone, a velocity eual to 0 at the wall would break too much the flow (think that the velocity profile is in reality logarithmic, whereas in finite elements it is linear, which near the wall gives less flowrate).

Regards,

JMH

Good morning,

I agree with that now but should'nt the nodes be set just behind the wall so it would be more "physicaly correct" ?

Another question : why don't we use this wall model all the time ? I can see in all of my corner's model (90 °) that there is not enough flowrate and that their influence is too strong. I will probably change the boundary condition for my next run (12 h each) and see how it changes the results.

Hello,

When the mesh size is rather large it is better to discard completely the boundary layer and apply just a no slip condition.

Beware with the boundary conditions in corners between solid and liquid segments, points must be declared liquid here, as a liquid segment must be between two liquid points.

Regards,

JMH

Thank you for responding the questions.

Regards.