open TELEMAC-MASCARET The mathematically superior suite of solvers

I have tried to make some runs with telemac2d, but I usually got a message during the calculations as follows:

Ill posed Problem, entering free velocity

Sometimes the software continue the calculations and sometimes it stops without reaching the end.

Can someone tell me what this message means.

Hello,

This message means that in an exit where you declared free velocities, some of these velocities are entering the domain (this is the case when a von Karman eddy exits a domain). In this case there is a risk that these velocities grow to infinity (and it will still be a solution of Saint-Venant equations), the problem is not well posed in the sense of the theory of characteristics.

The solutions in this case :

* if you are in a tidal computation : choosing a domain which is large enough, so that the depth is maximum at such boundaries.
* in fluvial conditions : this happens more seldom, except when there are von Karman eddies, and generally in this case it works.
* adding a local friction that will slow down spurious velocities, but well, this also changes physics.
* applying Thompson boundary conditions.


With best regards,

Jean-Michel Hervouet

I am Modeling a river estuary where I stop just at the end of the river. I got the problem of 'ill posed problem' when I introduce a sine wive at the exit or when I make variable water level (by liquid boundary file, an increase in the water level for one meter in 10 hours then decrease) or even when I impose salinity at the exit by specifying prescribed value for salinity.

So, which of your recommendations do you think is better in my case

Hello,

In your case your problem is not well posed when the elevation increases at your boundary, which triggers entering velocities. In our studies we use the Thompson boundary conditions. There is nothing to change in your parameter file except the keyword :

OPTION FOR LIQUID BOUNDARIES (OPTION POUR LES FRONTIERES LIQUIDES)

which is by default 1;1;1;1.... (as many as liquid boundaries)

and that must be now :

1;2;1;1... assuming that your offshore boundary is number 2.


With best regards,

Jean-Michel Hervouet

I did it and it worked fine for the boundary near the sea, but know I get a new error at the other boundary, the error message is:

'Provide velocity profile or check water depths'

Do you think that this is problem of slow flow (the velocity in my case is 0.1 m/s), or it is something else. At this boundary prescribed water flow is given and the boundary conditions set to be imposed flow and free water depth.

Hello,

This is something else. You prescribe a discharge at a boundary, and for some reason there is no water left on this boundary (initial condition ? tide ?). Then the program finds that even if putting infinite velocities the discharge will always be zero. I suppose that this boundary is the river upstream the estuary. A solution is to put an artificial bottom elevation at this entrance (dig a hole !), so that there is always water, whatever the tide. Another solution would be to put an imposed elevation of water, but this is more tricky if the level inside the domain does not correspond to this elevation (it would do a cascade...).

If you have dry zones on this entrance, look also at the different options for setting a profile :

VELOCITY PROFILES (PROFILS DE VITESSES)

in your case option 4 or 5 (new in version 6.1) would be the best.

With best regards,

Jean-Michel Hervouet