open TELEMAC-MASCARET The mathematically superior suite of solvers

I'm trying to model an estuary in Telemac 2D and I'm still having problems with enormous water velocities entering the model at the seaside boundary. At the seaside of the model I insert a 'surface libre' boudary condition of a measured tide. With the same mesh a first run resulted in a good simulation with acceptable results. When I redid the simulation I only changed the friction coëfficient (Manning from 0.025 to 0.02) and I got this plume of very high water velocities entering at the boundary. I had this problem before and it seems to me that with different simulations this 'plume' occurs at different locations of my boundary. So this would mean that the bathymetrie or the shape of the boundary has nothing to do with this.
I attached an image file to give an idea of what I'm talking about. the red colour indicates values up to 80m/s.

Has anyone experience with this problem?

Dear Svensmolders

This problems is linked to the type of boundary condition. In you case, you impose a water level varying in time (on a large boundary), and this problem occur when the level rise (some water is entering in the model).
In those conditions, the velocities are free, that's why you could obtain locally such important values.

The origin of the problem is related to some inconsistencies between a constant water level imposed on the boundary and the propagation inside your model.
Sometimes it works without any problem (like in your case with manning 0.025) and sometimes it crash. In the second test it may indicate that the imposed water level is inconsistent with this friction value...

For such problem, one solution is to prescribe also the velocities and using Thompson method at the boundaries or to prescribe water level varying in space (in accordance with the internal propagation).
If you seaside boundary is large, the best solution is to extract the boundary condition from a large model (But that means you should have such large model or buy such boundaries conditions ...)
Where is your estuary?
Christophe

Hello Sven,

This is a classic case of boundary conditions which are not well posed. When you prescribe free surface elevation and that entering free velocities appear on the boundary, this is also a solution of equations and you cannot complain because you said that the velocities were free (in fluvial flow we miss an information). The known solutions to this very fundamental problem of fluvial open conditions are :

1) put the boundaries sufficiently offshore so that the depth is large and the velocities small. Then it appears to be stable.

2) add a local head loss or a friction (we did that successfully in Telemac-3D)

3) use Thompson boundary conditions (the only solution which is correct in theory). You prescribe depth and velocity as 5 5 5 and add the keyword:

OPTION FOR LIQUID BOUNDARIES : 1;2;1 (as many as liquid boundaries, and the "2" only where you want Thompson. Then Thompson takes what he wants in your data, depending on Riemann invariants theory.

We can discuss this in La Rochelle,

with best regards,

Jean-Michel Hervouet

Dear Christophe and Jean-Michel,

thank you for the quick reply.
What I did to reduce this problem earlier is to lower the bathymetrie or to create a larger depth. I used a depth on this boundary of 50m. This seemed to work fine, but in this latest simulation with the 4th high water it crashed as shown in the picture above.
I understand the problem of the computation. I will try the Thompson and I will see if I can get boundary conditions from a bigger model. I know it exists.
The estuary I'm working on is the Scheldt (l'Escaut)in the Netherlands and Belgium.

I will prepare a little presentation on my case for the user conference in La Rochelle.

regards,

Sven