open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi all!

I have a T3D model that crashes because of planes 1 and 2 crossing each other at a given point at the bottom. The model crashes after 15 time steps when I run it when applying a locally increase air pressure to model. The model runs fine without this extra pressure.

A similar model, with similar set-up (extra air pressure) but a slightly different mesh, was not crashing.

I have tested the following, but the problem remains:
TIDAL FLATS = YES
BYPASS VOID VOLUMES = YES
NON HYDROSTATIC VERSION = YES (I have no as default)
OPTION FOR THE TREATMENT OF TIDAL FLATS = 2

I attach my files.

I use verion 7p1r0.

Thank you very much in advance for your help!

Best regards
PL

Hello,

It would be interesting to know what says the program on the planes intercrossing, is it by a large distance or a very small value ? Is it on a dry zone ? This is to know if we are just facing a truncation error in subroutine calcot.f or if it is another kind of bug. As a matter of fact in parts of calcot.f we already had to carefully manage truncation errors in formulas to avoid "intercrossing" that are only planes touching themselves.

Anyway I would need all the files to run the case and see what happens exactly, I do not see an obvious error in your Fortran and steering files.

With best regards,

Jean-Michel Hervouet

Good morning!

This is the error message:

With 6 mm difference it doesn't look like a truncature problem, does it?

Anyway, I attach all my files, would be great if you can try to have a look at it.
In parallel I will try to modify sligthly the mesh and see if I can go around the problem.

Thank you in advance for your help!

Best regards
PL

PS: I send you the case by email, I can't upload the files...

Hello,

No, the question is how you can have a negative depth of - 6 cm with the treatment of negative depths set to 2, that should prevent this. The source with a negative discharge is probably the guilty one. You can try to add subroutine positive_depths in your Fortran file and after the message "NOW THE NEGATIVE SOURCES" you will see the depth modified by lines H%R(I)=H%R(I)+... (done twice depending on OPTSOU). You can add after a line H%R(I)=MAX(H%R(I),0.D0) and it should cure the problem. However the mass conservation will not take this into account and will be wrong. I do not really know what to do when a negative source is imposed on dry land. Probably some preliminary limitation like we do for evaporation.

With best regards,

Jean-Michel Hervouet

Hello,

Thank you. I have tried it, but as you mention, the mass balance is spoiled.
My negative source is located at 2 m depth and at the crashing point the total depth is 17 m. I wouldn't have thought that such a high source could lead to such a problem on the bottom.

And once more, the model crashes only when I apply the extra air pressure - in mormal conditions it runs fine.

I thought that it could come from the vertical mesh since I use mainly fixed elevations (exept near the bottom where I have a sigma transformation between planes 1 and 3, to allow for more vertical flexibility in deeper areas).

Another thing is that I theoretically don't have any tidal flats in my model (bottom is always lower that free surface). However it crashes with TIDAL FLATS = NO. Is it something to investigate?

I will also try by slightly changing my mesh, hope I can come around the problem this way.

Best regards
PL

Hello,

I had not noticed TIDAL FLATS=NO and you should try with YES, so that the positive_depths algorithm is applied, however it may still crash due to the negative source. As the negative discharge is applied at one point it may trigger a negative depth is the volume of the point is less than the quantity withdrawn, i.e. if the integral of 2D test function * the depth is pumped in a time step. So reducing slightly the time step could be also a solution. Of course refining the mesh at that point is NOT the solution, as the total volume carried by that point would decrease, increasing it would be more sensible.

With best regards,

Jean-Michel Hervouet

Hello,

Sorry, I was maybe not clear. I do have TIDAL FLATS = YES but tried with NO (I had it working with NO with a 0,6 m higher water level).

I am testing now with positive_depths and as you mentioned, the mass balance becomes very poor.

Will try by changing the mesh, slightly looser resolution around my negative source. Can also try a lower time step.

I will give feeback.

Best regards
PL

Hello,

A slight decrease in the mesh density around my water intake node (7 m instead of 5 m) seems to do the trick!

The model runs fine, fingers crossed.

By the way, thank you for implementing the user variables reading function in the geometry file, it makes life so much easier!!

Finally, I am also pleased to see how well the model runs with a locally increased air pressure (1,62 m negative shift on only 1 m horizontal distance)...

Best regards
PL