open TELEMAC-MASCARET The mathematically superior suite of solvers

My computations involve sudden change in flow in the upstream cross-section of a rectangular canal. Flow rises from steady-state to a larger value and changes back to steady state (triangular hydrograph). After peak passes downstream cross-section, flow falls below the steady-state flow (for some cases, water goes into domain from downstream section). Is there any way to resolve this?

It could be that the prescribed elevation at the exit is too high and no longer relevant to the exiting discharge. As a matter of fact, in real conditions the water level at the exit of your domain evolves with the discharge. A solution could thus be to use a depth-discharge curve (see explanations in the telemac2d version 5.9 update).

Another solution would be to put more diffusion.

Another solution would consist of adding an extra length of channel at the exit, with larger depth so that at the exit the flow is more settled and has a correct profile.

Another point would be that you have high slopes at the exit, with tidal flats, this is not so well posed as flow may be supercritical in this case.

I hope something helps among these hints,

Jean-Michel Hervouet

Prescribed elevation at the exit is equal to steady-state water-level and remains constant during computation. I know that this is very rigid BC but that wasn't supposed to give problems.

I could increase diffusion but since I'm comparing TELEMAC-2D results with the results or another numerical model, this step should be avoided. Geometry modifications were also on my mind but didn't consider it for the reason above.

The problem is composed so that only sub-critical flow occurs.

I think that the source of this is the treatment of boundary condition. I would like to prescribe the directions and let TELEMAC-2d compute only intensities (and restrict them to be positive). Is there any way to restrict the directions of velocity vectors along a BC?

Well actually there is no specific boundary condition treatment at an exit with free velocities. We only check if velocities are re-entering and put a warning that you probably see. Would you like to do corrections, you could insert subroutine propin_telemac2d into your FORTRAN FILE. Then after line ALERTE1=.TRUE. you can try to change U(N) and V(N), provided that you change their INTENT(IN) into INTENT(INOUT). We have such a case in the so called pildepon case, in the wake of a pier, and this is normal.

You can try also to change the advection solver for velocities. It is the first figure of keyword :

TYPE OF ADVECTION

1 is characteristics
2 is SUPG
4 is distributive scheme
etc.

If you have 1 (default) try 4 which is more diffusive. We are happy with characteristics because with them we have von Karman eddies behind bridge piers and correct oscillation period, whereas with more diffusive schemes like finite volumes with first order, you find no eddies at all, which raises no problem at exits but is not really physics.

Regards,

JMH

Available advection schemes are (according to reference manual):
1-Method of characteristics
2-Centered semi-implicit scheme + SUPG upwinding
5-Conservative scheme + SUPG
6-PSI scheme
7-N scheme

There is no mention of option number 4. Am I missing something?

Yes, what we miss is the new user manual relevant to version 6.0 (soon). But you can see it in the telemac2d dictionnary in directory lib, under TYPE OF ADVECTION keyword. Regards, JMH

Explanations on new advection schemes are also in the file enclosed. I don't see it in the download section, though it should be here.