open TELEMAC-MASCARET The mathematically superior suite of solvers

Tried T2D scalar and parallel - no problems
T2D + TOM in scalar and parallel - no problems

As soon as I add the coupling with SIS the simulation stops.

I attach the std_out and what comes back from the debugger below. I can not see what causes the problem and would be happy get help.

Thanks in advance
- Clemens

Hi Clemens,

The error seems to appear during sisyphe execution. What happens if you try a T2D-SIS simulation (without wave effects) ?
For a sequential run, set PARALLEL PROCESSORS = 0 (I think you need a sequential version of the executable, compiled without mpi librairies).

Regards,
Laurent

Hi Laurent,
it ends with the same error.

Regards,
Clemens

It also crashes during the call to CONLIT subroutine?
If beforehand, you succeed in running the test cases provided with telemac installation, can you provide this T2D-SIS case please?

Hi Laurent,

Attached are the two files. I used the scalar version to run it.
AS written before the example cases work without any problems both in scalar and parallel.

Regards

Hi,

Can you also provide your geometry, cli and liquid files please?

Yes of course.

You will find them attached.
I changed the ending of the liquid file to .txt from .lic to be able to upload it.

The boundary conditions file is missing

Ohh sorry.

There you go

Clemens,

I tested your case with v7p3r0 and with a scalar execution (executable compiled without mpi libraries and parallel processors = 0).

From the second iteration, the hydro solver doesn't converge (NaN values appear). After some investigations (I ran your case in offline mode: T2D first and then SIS with hydrodynamic file from previous T2D computation) I found that you're prescribing no bottom elevations on your liquid boundaries (LIEBOR=2 wall conditions in your *.cli file) that lead to an incompatibility during the resolution of mass conservation over these boundary nodes. If you set LIEBOR=4 (free bottom evolutions), your case runs fine.

I strongly advice you the improve the resolution of your mesh near the river boundary and check the global quality of your mesh (it contains many weird elements, able to trouble the run).

By the way, your sisyphe steering file contains both BEDLOAD and SUSPENSION processes. For bedload computation, you're using Soulsby/Van Rijn formula which already accounts for suspension effects, so you're considering it twice by turning on SUSPENSION too. I advise you to turn off the suspension, or to choice another bedload formula that does not account for suspension effects.

I hope it helps.

Regards,
Laurent