open TELEMAC-MASCARET The mathematically superior suite of solvers

Dear all,

I am modelling a part of an estuary (about 60km) with Telemac3D. I have 2 open boundaries, both of them under tidal influence:
- downstream boundary: imposed water level (5 4 4)
- upstream boundary: imposed flowrate (4 5 5)

The downstream boundary is about 3300m wide, while the upstream boundary is around 10 times smaller. I use OPTION FOR LIQUID BOUNDARIES = 1 for both boundaries. In order to get rid of some higher flow velocities at the downstream boundary, I deepened the bathymetry here locally.

The model runs ok, however when I check the results I see that there is water recirculation at the downstream boundary. Often, water is flowing in the model at one end of the open boundary while water is flowing out of the model at the other end of the boundary. At the upstream boundary no problems occur.
Can anybody give me advise on how to avoid this effect? Do I need to use a different boundary condition or are there numerical parameters I can use to suppress this effect?

Thank you very much for your advice!

Best regards,
Stefaan

Hello,

Your problem is not well posed at the downstream boundary when the flow gets in (and the recirculations you observe are one of the many solutions). The usual solution is to use the Thompson boundary condition for this boundary (OPTION FOR LIQUID BOUNDARIES = 2;1 or 1;2 depending on the boundary number), and to give the elevation and the velocities if you know them. If you do not know them let 5 4 4, and the theory of Thompson will find values based on Riemann invariants.

With best regards,

Jean-Michel Hervouet

Dear Jean-Michel,

Thanks for your reply. I used the Thompson boundary condition as recommended and the results are better. The recirculations are gone and the in- and outflow is more realistic, however still not 100% satisfying. As an example I attach a screenshot of the downstream boundary during inflow. It is strange that inflow is only occuring at certain parts of the downstream boundary, while the flow velocities are perpendicular to the boundary at other locations.

I also noticed a negative effect of the Thompson boundary conditions related to the water levels. At the boundary nodes, the water levels do correspond with the imposed water levels. However, from the downstream boundary condition 1 node inside the model domain the water levels are already different (see figure in attachment: blue line = imposed water levels; green line = water level 1 node inside the model). The low water levels are ok, the high water levels deviate a lot. Did you already experience the same? Do you have any idea how to overcome this problem?

I deepened the most downstream part of my model to 50m below sea level, to get rid of very high inflow velocities. Is it possible that this has to do something with the strange results?

Thank you for you very much appreciated feedback.

Best regards,
Stefaan

Hello,

I enclose a variant of subroutine thomson which performs better on difficult cases, provided very recently by Michael Turnbull of HRW. It also requires changing bord.f in 2D but can work as such in 3D. It will be a second chance. You can also see in subroutine thomps_2dto3d.f (library telemac3d), there is a hardcoded option setting 3D velocities constant on the vertical for Thompson boundaries. You might want to test the option 2, setting a logarithmic profile.

Anyway high inflow velocities are always a problem on such open boundaries.

With best regards,

Jean-Michel Hervouet