open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

Hum, it is a problem of Python that decides that it is not called in the library and does not have to compile it. So take the subroutine (in bief) in your Fortran file, there it will be compiled.

regards,

JMH

Thank you very much Jean-Michelle, I got it. It has compiled fine, but if run fails then it should indicate the guilty variable. I will update you tomorrow. Thanks again.

Kind Regards!

Violeta

Dear Jean-Michel,

Thank you for your advice. I run my case with CALL CHECK_DIGITS but got the same output as before. It did not really indicate what variable is guilty. I have attached the two output files here, maybe there are more info that I missed. In mean time I will try to run this case on cluster but just on one processor, but it is not a solution as it would take ages to complete, if it completes. Let me know if it is ok with you and I will post all my files to the case, if you would like to run it, when you get a minute. Thank you very much.

Kind Regards!

Violeta

Dear Jean-Michele,

Please see attached all files for this case which gives me the Characteristics Intersect >99 error. I managed to run similar case in parallel with time step 1sec but with higher time steps it fails. I have used CALL CHECK_DIGITS but it did not point to any variables. Sorry to annoy you but would you be so kind to take a look at my files and point me into right direction. Thanks in advance.

Kind Regards!

Violeta

Sorry, but files were too big to post them. So I have the link here with all the files for the case. Thanks a mil.

we.tl/9iI424kEVS

Kind Regards!

Violeta

Hello Violeta,

I got the files and started to run the case. However it stops in the characteristics after only 60 time steps, is it what you observe ? I would like to make sure that it is a problem in the characteristics or in parallelism and not simply a problem of numerical stability. If you tell me that other advection schemes have the same behaviour, I am not so sure.

Regards,

Jean-Michel

Hello Jean-Michele,

Thank you very much for looking into it. Yes, I have tried all available Schemes for advection of velocities and most of them did not even run or stopped after few time steps with same error message. The only Scheme that works for me is Method of Characteristics. For this case the run stopped after 840 times. But if I use another Advection scheme then maybe I need to change other parameters as well that I did not do, then it might work as different combination, but I used the Steering file as it is just changing Scheme and it did not work. But it works with 1 second time step right now, just it is very slow. Please advise. Thank you.

Kind Regards!

Violeta

Hello,

Well described like this it is only a problem of numerical stability, not a hint that there is a problem in parallelism. I'll do some tests and I'll report.

With best regards,

Jean-Michel

Thank you very much Jean-Michele for your help. Let me know what to change and I can run experiments too and let you know if any errors. Thanks again.

Kind Regards!

Violeta

Hello,

A first report. The case was indeed very unstable and I got something that seems to work, but do not have the results yet. It may take time to sort out what is important, I changed various things :

* initialisation of tracers : it is better to work on elevations than plane numbers because the elevation of a plane may be varying on high bottoms. Example for plane 19 do a test IF(Z3%R(J).GT.-200.D0) THEN... You have the same problem in TRA_PROF_Z.

* Preconditioning 17 does not seem to like the tidal flats, so I changed 37 into 2 and 17 into 2. The solver for PPE could probably be GMRES (7), not tested.

* I removed k-epsilon and put 2 for vertical turbulence model. Then I set the
COEFFICIENT FOR HORIZONTAL DIFFUSION (OF VELOCITIES and OF TRACERS) at 2.D0.
Beware, when you have k-epsilon on the vertical it is set also on the horizontal and in this case your value of 0.1 for horizontal diffusion of velocity is wrong, it should be 1.E-6.

* I removed the hydrostatic inconsistency filter (it seems important, though it was here to help... surprising)

* I have set all advection solvers to 14.

I try to have the case working with a time step of 60 s, just to see, but maybe we will have to choose a smaller one eventually.

This is all for now,

Regards,

Jean-Michel