open TELEMAC-MASCARET The mathematically superior suite of solvers

When running TELEMAC 2D the program is printing this message at the compulation of every time step:

EQUNOR>BIEF>: EXCEEDING MAXIMUM ITERATIONS: 100 RELATIVE PRECISION 0.17134

ILL-POSED PROBLEM, FREE DEPTH ON BOUNDARY WITH ENTERING VELOCITY AND SUPERCRITICAL FLOW.

I am running a steady flow with imposed flow at the inlet and a velocity profile for u.

The program is running all time steps but at the end I see only the water depth at time step 0 (initial condition?) The result layer in FUDAA post-processsor is only showing one time step (the time step 0)

Can anybody tell me what is going wrong? Is there any way to know whether the results for all time steps are really generated or not?

Hello,

Here are a few hints:

You are probably running Telemac with defaults values of parameters, some of them can be improved (and are kept as such in the defaults values for the sake of already existing test-cases and old studies).

I would advise to have in your parameter file:

TREATMENT OF THE LINEAR SYSTEM : 2
SOLVER : 1

Then the wave equation will be solved instead of the primitive equations, it will be much faster. Then the conjugate gradient is OK and solver=1 is possible.


Then check the key-word : PERIOD FOR GRAPHIC PRINTOUTS
this is probably the reason why you see nothing in your results file.

You should then look at the outflow boundary conditions, where you should have a prescribed depth (or elevation) condition. On this outflow the velocities are free and it may be that a few velocities will enter the domain (this is so in the test-case called "pildepon", when a von Karman eddy exits). At the lines corresponding to the exit the boundary conditions file must start with 5 4 4, stating that depth is prescribed and U and V are free.

The parameter file can be changed with Fudaa but once you are used to keywords you can also edit it as a text file.

I hope this will bring some improvement,

With best regards,

Jean-Michel Hervouet

Jean Michel
Is there a problem of time step also ? if the maximum of iterations is reached, maybe he should take smaller time steps.
Kindly

Hi Jean,
Thank you very much for your reply. Since I ultimately want to simulate a flood condition (unsteady event) I thought it won't be good to prescribe a constant water surface elevation at the outlet. So I created a quite deep artificial lake (it will take lot of water to fill in) at the entire outlet boundary. So I was running the model with only one liquid boundary (i.e. the inlet). Is it possible that TELEMAC is not liking it?

Shall I discard the artificial lake? I have no data for the outlet, how to prescribe a value?

Kindly suggest something. In the meantime, I am trying to follow your suggestion.

Joy

Hello,

If you have an exit boundary without any data, that may be reached by water, a possibility is to choose an incident wave boundary condition : 1 1 1 in corresponding lines in the boundary conditions file. It will prescribe boundary conditions so that the Riemann invariants correspond to a situation without water on the other side of the boundary (if you start with no water here). However this may eventually influence your results if the exit has a fluvial regime. Putting free conditions (4 4 4) is more risky and may be unstable.

With best regards,

Jean-Michel Hervouet

Hi

To avoid the cases where the regime is fluvial, you can modify your the bathymetry at the outlet of domain such that the flow at the exit is always torrential.
You can for instance, add few elements to your mesh at the exit (a basin) and prescribe a highly decreasing slope in the bathymetry.
I hope that this can help.
Kind regards

R. Ata

Thanks. Just a quick question. I ceated a vriable named BOTTOM FRICTION in Blue Kenue and mapped the manning's roughness coefficient into that mesh and saved it along with BOTTOM (containing the elevation) as a SELAFIN file.

How can I be sure in terms of keyword selection that TELEMAC is reading the manning's n from the geomery file and more than that, how to tell TELEMAC that the variable BOTTOM FRICTION in the geometry file is actually containg Manning's roughness coefficient not Chezy or something else.

Thanks and regards,
Joy

Hello,

The bottom friction is recognised by its name in the file and somewhere in the listing you should find :

FRICTION COEFFICIENTS READ IN THE GEOMETRY FILE

then the friction law must correspond to the kind of coefficient you have given, there is no security at this level.

Best regards,

Jean-Michel Hervouet

Hi,
I ran the program by mentioning the SELAFIN file (that contains both BOTTOM and BOTTOM FRICTION) as the previous computation file. Then I set the keyword LAW OF BOTTOM FRICTION to 4 (corresponding manning) and run the program. I did not alter anything in the keyword FRICTION COEFFICIENT (the dafault value is 50) assuming that the program will read the friction coefficient from the PREVIOUS COMPUTATION file.

But unfortunately the program immediately stopped saying

THE LAW OF BOTTOM FRICTION 4 IS ASKED
GIVE THE CORRESPONDING FRICTION COEFFICIENT

What am I doing wrong? The program is still expecting the friction coefficient from the FRICTION COEFFICIENT keyword instead of the SELAFIN FILE.

Any help will be very much appriciated.

Hello,

You are starting a new computation and Fudaa treats the initial conditions as a previous computation file, this is perhaps the origin of the problem.

I suggest that you put in your parameter file :

COMPUTATION CONTINUED : NO

and that what was before the PREVIOUS COMPUTATION FILE is given as the GEOMETRY FILE

You can then suppress the keyword PREVIOUS COMPUTATION FILE in your parameter file.

This should work better as the friction coefficient is first looked for in the geometry file.

With best regards,

Jean-Michel Hervouet