open TELEMAC-MASCARET The mathematically superior suite of solvers

Hope this uploads this time!

Ah the geometry file is too big to attach. Do you use one drive, perhaps I an share it on there?

If you put it somewhere where I can download it, I may manage to get it. Just tell me where.
Liquid boundary file is OK/

Great, try this...

bangoroffice365-my.sharepoint.com/:f:/g/...Lu_w_2oALAw?e=qySS1l

Thanks again,

Neil

Hello Neil,

I have found the problem with your model.
It is because of the number of tracers you model (10) and the use of 2 features:
- characteristics in parallel for the advection schemes (that is what I told you, so it is still needed to use SCHEME FOR ADVECTION OF TRACERS=5;5;5;5;5;5;5;5;5;5 + SCHEME OPTION FOR ADVECTION OF TRACERS = 4;4;4;4;4;4;4;4;4;4) rather than the default values. Anyway, as told before, they are better to simulate tracers and conservation of tracers,
- Thompson conditions for the computation of the boundary conditions. I would advise to use the default value for OPTION FOR LIQUID BOUNDARIES = 1;1;1;1;1;1;1 or simply comment your current line with this keyword (the number of values equal to the number of liquid boundaries is automatically filled by TELEMAC-2D if you do not write the keyword OPTION FOR LIQUID BOUNDARIES).
In that case, you may have to change the code 5 6 6 (i.e. prescribed water depth/elevation and velocities) in the BOUNDARY CONDITIONS FILE to 5 4 4 (i.e. prescribed water depth/elevation and free velocities) and let the code for tracers at 5 as you have done.

With that, I think you should enter and start your simulation.

Chi-Tuan

Hello Neil,

After reading more deeply the sources, if you still want to use the Thompson boundary conditions for your case, can you try to copy the following subroutines in your FORTRAN FILE (use a folder rather than a single concatenated file) and change a few lines with the value 14 rather than 10:
- declarations_parallel.F with DOUBLE PRECISION :: BASKET(14) ! VARIABLES INTERPOLATED AT THE FOOT
- org_charac_type1.F with INTEGER, PARAMETER :: MAX_BASKET_SIZE=14
- streamline.f with INTEGER, PARAMETER :: MAX_BASKET_SIZE=14 ! LARGE

The enclosed steering file with your input files work for a few time steps here.
I used the European Shelf local solution rather than the global TPXO solution as I do not have the last one, but it should not change your issue of MAX_BASKET_SIZE (but your tidal results may be better).

My main changes are:
FORTRAN FILE = user_fortran
with the 3 modified subroutines
SCHEME FOR ADVECTION OF TRACERS = 5;5;5;5;5;5;5;5;5;5
SCHEME OPTION FOR ADVECTION OF TRACERS = 4;4;4;4;4;4;4;4;4;4
and
OPTION FOR LIQUID BOUNDARIES = 1;1;1;1;1;2
rather than
OPTION FOR LIQUID BOUNDARIES = 2;2

I am not sure that you really want to use the Thompson boundary conditions with your open boundaries with prescribed flowrates, perhaps only for the maritime boundary.

Please tell me if this works for you.

Chi-Tuan

Thank you so much Chi-Tuan - I am very grateful for your input. Unfortunately I am unable to test it today but I will do as soon as I can and will let you know.

Kind regards,

Neil

Hi Chi-Tuan,

Your advise was spot on and I managed to get this to run today so thank you very much for your help!

Next step is to integrate some water sources to introduce the tracers but hopefully that shouldn't cause too many issues.

Best wishes,

Neil

Hello Neil,

That is good news. Thanks for your feedback.

Chi-Tuan

Hi again,

I have now tested the model with water sources - it works with 8 but then not with 9. It just fails to run without any details:

runcode::main:
:
|runCode: Fail to run

I understand that the MAXIMUM NUMBER OF SOURCES is set to 20 as a default and this can be increased but this is not the issue here. I have tried searching for solutions to this haven't been able to find anything - could this be related to the issue I was having with the number of tracers in parallel? Do you have any suggestions to try?

Many thanks,

Neil