open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi

I have been trying to use Telemac 3D for a hydrodynamic simulation with temperature (Power Plant Discharge). Initially my simulation was taking forever to run. After making some changes to the case file, now it's running. However, after the first day of simulation I get the following error message.

TRACER 1
ADVECTIVE FLUX THROUGH BOUNDARIES OR SOURCES : -150.2543
DIFFUSIVE FLUX THROUGH THE BOUNDARIES : 0.000000
MASS AT THE PREVIOUS TIME STEP : 0.1397576E+10
MASS AT THE PRESENT TIME STEP : 0.1397576E+10
MASS EXITING (BOUNDARIES OR SOURCE) : -751.2715
ERROR ON THE MASS DURING THIS TIME STEP : 528.9401
MURD3D: ITERATION NO. REACHED 100 , STOP.
ALFA = 0.152446384061269
GUILTY POINT = 1

The water mass balance is fine. I am attaching my case file and the output file.

Thanks in advance

Viviana

Hello,

Have you tidal flats ?

If yes, as it seems, use also scheme 14 for advection of tracer, and it is probably the reason of the crash and the mass-balance which can be much better (scheme 5, the PSI scheme, does not work for elements with no volume). The sub-iterations of scheme 5 for getting stability are certainly hindering a lot the computation.

The solver for diffusion of velocities can be 1 (conjugate gradient) instead of 7 (GMRES, sophisticated for difficult non symmetric systems) and it will probably be faster.

With best regards,

Jean-Michel Hervouet

Hi

Thank you for your suggestions. I do have tidal flats and I have changed the advection of tracer to 14 and the solver for diffusion of velocities to 1. But I got the following error at the 24 hours of simulation:

GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 500 RELATIVE PRECISION: 0.1332847
GMRES (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 250 RELATIVE PRECISION: 0.1444819E-05
GMRES (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 250 RELATIVE PRECISION: 0.1983786E-04
GMRES (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 250 RELATIVE PRECISION: 0.1458820E-01
GMRES (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 250 RELATIVE PRECISION: 0.7966080E-03
GMRES (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 250 RELATIVE PRECISION: 0.1018514E-03
GRACJG (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 500 RELATIVE PRECISION: 0.7466739E-01
GMRES (BIEF) : EXCEEDING MAXIMUM ITERATIONS: 250 RELATIVE PRECISION: 0.1194800E-01
DEBIMP3D : PROBLEM ON BOUNDARY NUMBER 2
GIVE A VELOCITY PROFILE
IN THE BOUNDARY CONDITIONS FILE
OR CHECK THE WATER DEPTHS

So, I reduced the time step from 5s to 2s, but the simulation is taking too long so I haven't been able to checked the new results in the output file.
I don't know if I have something else wrong in my domain.

Thanks again for your help

Viviana

Hello,

Now you've got to find out what happens on boundary 2 after 24 hours of simulation (getting dry ? oscillations ? open boundary with problem not well posed ?).

Regards,

JMH

Hi Jean-Michel,

I am working on an estuary model with salinity as tracer. The model works when I set SCHEME FOR ADVECTION OF TRACERS to 14 but crushed within a few time steps when I set it to 5.

On this post, you suggested to try Scheme 14 for advection of tracer. On the other post (www.opentelemac.org/index.php/kunena/21-...ity-appears-suddenly) , you mentioned that ", the method of characteristics is unconditionally stable, with monotonicity, it can deal with tidal flats without stability problems, but it is not mass-conservative, so I use it only for the advection of velocities, and also k and epsilon."

Can you clarify a bit on the applicability of Scheme 14 for tracers? Thanks.

Edwin

Hello,

All what you report is quite normal, if you have tidal flats. Scheme 14 is an adaptation of the distributive N scheme to tidal flats, it does sub-iterations so that it appears, from a user's point of view, unconditionnally stable, it is mass conservative and monotonoous, exactly what we want for tracers. Scheme 5 is the distributive PSI scheme, which implies divisions by the volume of elements in the algorithm, so it will not work on tidal flats (though we can make it work in some special cases, e.g. with crushed elements with a volume exactly equal to 0, while other elements will have a volume clearly greater than 0, in which case a test on volume can easily be done).

Scheme 14 is described in the release notes of version 6.0. It has been published in the proceedings of the IARH conference in Brisbane in 2011.

With best regards,

Jean-Michel Hervouet

Thanks for the explanation.


Edwin