open TELEMAC-MASCARET The mathematically superior suite of solvers

Greetings Telemac community.

We are running into issues with random boundary instabilities in a Telemac2D tidal model. One out of three times we run the model it will run is fine no instabilities. But we often find that the model goes unstable at the offshore boundary. It seems that the instability is related to the model partitions and we can move where the model goes unstable (at the boundary) by changing the number of grid partitions we use. We are currently using the Trunk version of the code but have also tried v8p2. The grid consists of 1.8M nodes (~3.5M elements) and we see a computational speed-up up to 400 CPU's. We have tested the model with a range of time from 1-10 seconds, where a 4-5 second time step seems optimal.

Is there away to write out and re-use a partition file? i.e. Run the model until we get a stable result, then check to see what the grid partitions look like and re-use them in the next simulation? Or is there a better numerical scheme or solution we should be using?

Cheers

Hello Glen,

Can you clarify what you mean by "random" and "instabilities". By random you mean that it may depend on the number of cores you run the computation? Instabilities mean crash of the computation, spurious oscillations, strange results? Can you send figures please?

You can use some of the options available by the script telemac2d.py, see options with the hel[: telemac2d.py -h, in particular --split, then -x, then --run, and if you want to merge the different results file --merge. You will also have to use option -w.

Can you share your geometry file please? Or at least upload a figure of the extent + grid to see some coordinates values.
What about the size of the smallest elements? And the maximum velocities expected over the area?

Looking at your steering file (I would start with the 2 first items):
- the value COEFFICIENT TO CALIBRATE TIDAL VELOCITIES = 999 is very suspicious. You sould rather use a value around 1. (from 0.8 to 1.2 or maybe a little bit less or more) or the default value which means it is equal to the square root of COEFFICIENT TO CALIBRATE TIDAL RANGE (in that case, just comment the keyword line),
- have you tried not using the Thompson boundary conditions (OPTION FOR LIQUID BOUNDARIES = 1)? Without Thompson conditions, try to prescribe only water depth, over your maritime boundary first,
- what about the location of the point with longitude ; latitude = 180. ; -44. Is it around the center of your full domain? Can you show a map please?
- can you upload your different FORTRAN FILE + your BOUNDARY CONDITIONS FILE + your HARMONIC CONSTANTS FILE,
- why did you choose IMPLICITATION FOR VELOCITY = 1.0 and IMPLICITATION FOR DEPTH = 1.0? Why not the default values (= 0.55)?
- why did you choose SOLVER = 4? Why not = 1 (conjugate gradient?),
- have you tried to play with the keyword BOTTOM SMOOTHINGS?

Some other comments about your steering file but I do not think they will change your results (or change a lot):
- if you used a OSU tidal solution (like TPXO) or had to interpolate tidal constituents, you should use GEOGRAPHIC SYSTEM = 5 (Mercator projection) which is the geographic system at the moment when TELEMAC converts the mesh coordinates to longitude/latitude. When using spherical coordinates, at that step, it is the value expected by TELEMAC. But with this steering file, you do not face this step,
- VELOCITY DIFFUSIVITY = 0.5 may be quite big, how did you choose it?

Hope this helps,

Chi-Tuan

Hi Chi-Tuan,

Thanks for your reply, sorry for the delay in replying. I wanted to systematically test each of your suggestions.

By "Random instabilities" I mean that I see high velocities and odd water levels. Why I say they are "random" is that I can run multiple simulations and 1-3 times the results will exhibit no instabilities. Also the locations of the instability is inconsistent.

The model grid is in WGS84 lat/lon (0-360) and yes longitude ; latitude = 180. ; -44. Is around the center of the domain.

I have tried the default values for COEFFICIENT TO CALIBRATE TIDAL VELOCITIES and COEFFICIENT TO CALIBRATE TIDAL RANGE. This has made no difference.

I tried changing the from Thompson boundary conditions to OPTION FOR LIQUID BOUNDARIES = 1. This change caused the model to go unstable almost instantly. Can you use a Harmonic boundary file with OPTION FOR LIQUID BOUNDARIES = 1 or does it have to be a water depth time series?

I have set both IMPLICATION FOR VELOCITY and IMPLICATION FOR DEPTH to the default values this made no change to the boundary instabilities.

I have not tried bottom smoothing the FORTRAN FILE was CORFON.f where I was trying to see how bottom smoothing worked. I.e if you set BOTTOM SMOOTHING = 1 how aggressive is the smoothing algorithm.

I have changed for SOLVER = 4 to 1, the model now converges much faster. But we are still seeing jets of high velocities on the boundary.

Is it possible in TELEMAC to have a ring of high viscosity around the boundary to dampen these high velocities?

Cheers.

Hello Glen,

Do the high velocities start to appear at the boundary conditions? If yes, what about water depth at those locations?

Chi-Tuan

Hi Chi-Tuan,

Yes the high velocities are occurring at the model boundary conditions. The instabilities tend to move around so in some instances yes there are changes in the water depth and bathymetry. However, often the bathymetry is almost perfectly flat. In the attached figures the instability to the East at approximately -55,155. The bathymetry is almost consistently 4000m deep.

The two things which I have found will reduced the instabilities, are using a very high viscosity (0.5) and/or very low roughness (Chezy >80). The problem with this is its hard to justify using these values. I am in the process of testing bottom smoothing, I'm just not sure how aggressive and can reasonably go with this value.

Cheers

Hello Glen,

Can you upload your geometry file please, or at least the geometry file with the mesh with no bathymetry.

Chi-Tuan

Hi Chi-Tuan,

Sorry for the delayed reply. We have managed to get the model running without any instabilities. The solution was quite simple, I should have tried this earlier. The solution was to prescribed a velocity along with the harmonics to the boundary and the model runs flawlessly. Basically, what Telemac already does with the default TXPO boundary conditions.

Thanks again for all your help.

Hello Glen,

This is good news. Indeed, difficult to suggest this solution without seeing your BOUNDARY CONDITIONS FILE.

Chi-Tuan

Hi,

How do you prescribe velocity and water level? by describing 5 6 6 in the BC in Blue Kenue?

Hello,

The answer is yes in the boundary conditions file. Please read the TELEMAC-2D user manual.

If it is a Blue Kenue question, you should read or post your question in the Blue Kenue section. I cannot use BK.

Hope this helps,

Chi-Tuan