open TELEMAC-MASCARET The mathematically superior suite of solvers

Dear telemac community,

I'm trying to run a wet/dry beach suffering from erosion due to tidal surges (2m tidal range +80cm in extreme events). The beach has a jet that guides the navigation channel. The mesh has 3 borders (2 rivers with 15 and 7 m³/s) and the ocean. Since the study region is inside an estuary, a nesting was performed with a bigger mesh (macro.slf) where I run telemac3d v6p2r3 for 10 years, since hycom data is out of range.

Now for the micro-region mesh, I am using v8p1r2 with telemac3d and will later couple with Gaia/Sisyphe. In the region, altimetry data was collected with a drone and bathymetry as well. A fine mesh was produced and also friction coefficient was interpolated on the mesh. In the mesh, I considered 50m offset from the coastline as the solid border, while the region towards the water presents a decreasing positive elevation (with houses and trees).

The idea of this simulation is to analyze the sea level upwards the beach reaching the houses (and later on, the erosion related to this).

I'm having problems to run the micro mesh with topobathymetric data, even with fortran turned off. Tidal flats is on, I tried LEO POSTMA scheme and N-scheme and can't make it work. With time step equal to 2 I managed 12 minutes of simulation that crashed afterward with basically none free surface changes.

To run in v8p1r2 I based myself on two examples: bergenmeersen and tracer_wet_dry... But it led to no results at all.

For this scenario study, I need to run at least 1 year of results to properly evaluate dynamic changes, so the stability needs to be increased to use a higher time step, otherwise, the simulation will take forever to finish (I have 20 core only).



Thus summarise the numerical scenario and my questions are presented below, some may sound simpler but I'm not sure anymore where I might be inputting errors to the simulation.

1) What changes should I do in my .str to run with a positive level?
2) What is the proper method to impose boundary conditions (.dat) into v8p1r2, since I'm outdated in this matter.
3) I tried to convert .dat to binary (TelemacTools in Matlab and then conviee.f to convert to big-endian, is this really necessary?) but couldn't imposed using bergenmeersen approach. (data I needed to use is wind, air temperature, atmospheric pressure, while oceanic data are TPXO, sea surface height for 2d while 3d are current velocities, salinity and temperature for density law)
4) Which boundary conditions can be imposed using BINARY BOUNDARY DATA FILE? I've seen that TELEMAC reads the elevation, velocities U and V, and the values of the declared tracers. Does it also read atmospheric data or does it need to be in a separate file (with which variables? wind XY, air temperature, atm pressure all together?)?
5) Which fortran modules (and .str keywords) must I edit to make the data (binary or .dat) properly read?

The files are attached to this post.

Thanks in advance for any assistance!

Eduardo Kirinus

Hello Eduardo,
If I understand correctly, you have a larger model that fully encompasses this one. If that is the case, then you only need to setup boundary conditions on the large model and then extract timeseries of water elevation and velocities along the nested boundaries (BINARY BOUNDARY DATA FILE) and assign them to the nested one. There is a python module ('convert_to_bnd.py') that does the extraction.

Atmospheric (and any other 2D driving forces) do not apply to BINARY BOUNDARY DATA FILE as this defines condition at the boundary nodes only. There should be defined in their respective files.

There have been some bug corrections with BINARY BOUNDARY DATA FILE. So you either need to work with the trunk or wait for the next tag which is about to be released in a week or so.

As your setup is quite complicated, I would suggest to setup a simple nesting with just water elevation variation and if that works as expected, incrementally introduce other forcings or tracers. Troubleshooting would be much easier then. If you can post the setup of the encompassing model and the nature of the nesting, then we might be able to provide more help.

Best Regards,
Costas

Hello Eduardo and Costas,

Costas is (nearly) all right. Next official release (v8p2) is planned to be tagged in one month. Anyway, for the feature BINARY BOUNDARY DATA FILE, every current known fix has been committed in release v8p1r2, the one you are using.

Costas is really right when he suggests to start from a simple setting then add new features step by step for your local model.

Anyway looking quickly to your steering file + geometry file, 10 s may be a big time step with 1 m elements, depending on velocity.

What do you mean with:
- bergenmeersen approach?
- .str?

Hope this helps,

Chi-Tuan

Thanks for the answer Costas and Chi-Tuan.

Just to clarify some things, the uploaded file are already an "MWE" case, the mesh is 2km x 2km wide. None variables are added in those files as the fortran is turned off. The .cas imposes constant salinity and temperature in the mesh. My doubts remain regarding positive bathymetry and the proper configuration for tidal flats to work properly in my scenario, and if the errors occurring are related to it or other configuration.

@cyamin

Ok, so if I understand it correctly, the steering keyword BINARY BOUNDARY DATA FILE only works for water level and velocity (together in the same file? How telemac differentiate the variables?). How should Salinity and Temperature be imposed? as .DAT ?

For the imposition of ascii data, I must use the FORMATTED DATA FILE 1/2 ? Where should I put salinity and temperature as 1 or 2? Will the model imposes it correctly (nmesh*sigma*daily_time)? or should I edit the time spam read elsewhere?

Following your suggestion, I will add one variable at a time, after this scenario with no variables works.


@pham

Chi-Tuan, I need to run at least one year of this scenario, to get seasonal variations on the currents and tides. I was also testing with time step 1, but it seems too slow to compute the result. I estimated the courant number and for 1m elements, my time step should be something around 0,1 to 0,8 s (maximum velocity measured in the place shows 0,9 m/s, although the model shows 3-6m/s), so now I'm editing the mesh to increase to 3m elements to see if it works better and faster.

What I meant with “bergenmeersen approach” is that I used the bergenmeersen test case as a starting point to set up the simulation, as that case is (conceptually) similar to mine: It has the main watercourse and then the water level rises and floods dry areas.

I used the .cas file from the bergenmeersen test case, removed the drogues and culverts, added the temperature and salinity tracers, then added BINARY BOUNDARY DATA FILE to impose the boundary condition data. But this test also failed.

And .str is the file extension I used to use for the .cas file. I meant .cas.


######

So, In addition to my above questions, what do you guys think about the tidal flats with LEO POSTMA scheme? it is ideal for my case or should I use n-scheme?

Thanks in advance for all help and discussion!!

Eduardo Kirinus

Hello Eduardo,

You can use BINARY BOUNDARY DATA FILE feature with elevation, horizontal velocity components + tracers. You can have a look at the BORD3D subroutine to understand how it works. The name of the variable in this file determines the treatment at the boundary conditions (ELEVATION Z, VELOCITY U, VELOCITY V, name of tracers as defined with the keyword NAMES OF TRACERS).

If using ASCII input files, depending on if the boundary conditions varies in space and/or time, you can read the TELEMAC-3D user manual. If they depend on space and no standard treatment fits what you want, you will have to implement your treatments by yourself in USER_BORD3D e.g.
You can use IND_T and IND_S as index for temperature and salinity if you have given them TEMPERATURE and SALINITY as names of tracers. Otherwise, the numbering is the one given by NAMES OF TRACERS keyword.

To run faster, you may have to increase the minimum size of elements again. You can also try other advection schemes for velocities and k-epsilon, e.g. the method of characteristics (= 1), which may enable you to use bigger time steps.
For tracers, you need a conservative scheme that works with tidal flats. Schemes 13 and 14 work, you can also try LIPS scheme: SCHEME FOR ADVECTION OF TRACERS = 5 + SCHEME OPTION FOR ADVECTION OF TRACERS = 4.
If using schemes 13 and 14, be careful with the keyword MAXIMUM NUMBER OF ITERATIONS FOR ADVECTION SCHEMES. In release v8p1, the default value is equal to 10, but you should check that it is enough, see the message like:
MURD3D_POS SCHEME: 14 10 ITERATIONS
or
POSITIVE DEPTHS OBTAINED IN 10 ITERATIONS

and increase it if reached (from v8p2, there will be a message to warn if reached).

Classical Leo Postma (= 3), N type scheme (= 4) or PSI type scheme (= 5) should not work with tidal flats.

Quickly looking at your steering file, a few comments:
- depending on your bathymetry (if steep in particular), you may have to activate HYDROSTATIC INCONSISTENCY FILTER = YES,
- PRECONDITIONING = 34 (= 2 x 17) for every solver with conjugate gradient (SOLVER = 1) may accelerate your computation, except for propagation (keep PRECONDITIONING FOR PROPAGATION = 2),
- FREE SURFACE GRADIENT COMPATIBILITY = 0.9 is usually advised for real cases. You can also decrease the value up to 0 if you have spurious oscillations.
- I wonder why you activate DYNAMIC BOUNDARY CONDITION = YES?

Strange to talk about bergenmeersen approach when deleting culverts as this example goal is to validate this last feature. Anyway, you can also have a look to tracer_wet_dry example

What do you mean by "MWE"?

Hope this helps,

Chi-Tuan

Thanks, Chi-Tuan for the valuable keywords assistance.


About your questions, I have no clue why DYNAMIC BOUNDARY CONDITION was set to on, perhaps I forgot to turn it off in some test.

And MWE is Minimun Working Example... but in my case, it doesn't work

I will make some tests and reply later on.

Eduardo Kirinus

Thanks, Chi-Tuan and Costas for your valuable inputs.

Just to update the situation, the setup with tidal flats is now with a working .cas file, that seems to do the job pretty well, in addition, I made mild changes to the mesh (min. element = 3m), except that (as far as I can see) there are three (I hope) small issues.

The first is that Telemac seems to induce some sort of numerical
circulation near the border of the mesh (see the following picture).
This doesn't seem to affect (noticeably) the rest of the simulation, but
it still looks wrong. The circulation does seem to reduce in intensity
as the simulation advances, so it could be an initialization issue (I'm
initializing the simulation with zero current---should I not?). How can
I fix this (apparently) numerical-induced circulation? (see figure1.png)



The second issue is that sometimes near the dry zones Telemac3D computes
some crazy high velocities (for example, in the picture below), which I
think might be due to the wetting/drying process, but I'm just guessing.
How do I fix these spurious velocities? (see figure2.png)



The third issue, that is perhaps related to the first two, is that
Telemac3D seems to struggle to solve some equations (sometimes it's W,
sometimes it's k and ε, and sometimes the tracers (salinity and
temperature), but they often struggle to converge together). In the
attached .sortie file there are several occurrences of

which is the 1500 iteration limit I have set. Although it reaches the
iteration limit, it seems to recover fine from that. Regardless, I
would like to fix that, as this seems to be the performance bottleneck
of the simulation, as the rest runs pretty fast considering the size of
the mesh.

some files weren't attached

there is another way to share the files?

Hello Eduardo,
Unfortunately, not all file extensions are acceptable as attachments. But I think .zip is. Have you tried zipping all files together and posting the archive?

Regarding the first issue, this is probably due to poor boundary condition definition. In such cases, it is usually helpful to switch on Thompson boundary conditions (OPTION FOR LIQUID BOUNDARIES = 2;2;2 for 3 boundaries). More info in the manual (4.3.13 Thompson conditions).

Regarding the second issue, with TIDAL FLATS as water depth tends to zero, velocities skyrocket. There are things you can do to address this issue as described in the manual (6.6 Tidal flats) e.g. set a MINIMAL VALUE FOR DEPTH to something larger than the default.

The third issue I think is related to the second. Spurious velocities tend to hinder convergence.
All the above are based on my hands-on experience. Chi-Tuan can provide more insight.
Costas