open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello JR,

I do not know how you managed to run the model, but your case can't run with these settings!
- First, your liquid boundary file is not correctly formatted, I get an explicit error message during its reading at the first iteration of the model before stopping. You can have a look at the section 4.2.5 of the user manual and at the numerous test case.
- Second if you want to prescribe tidal signal on the east or north/east/south boundary, it concerns the 2nd liquid boundary, so in your liquid boundary file it's SL(2) and not SL(1) (that accounts for your river).
- Your initial elevation is not in agreement with the elevation prescribed at the east boundary. The model takes longer to initialize (small oscillations at the beginning of your run).
- For your river, you're prescribing both elevation and flowrate (5 5 5 code), is it really what you want? it's not really suitable, and usually, prescribing only flowrate is better (4 5 5). The quality of your mesh around this boundary is poor with flat triangles, you should improve it. Also, the bottom values on these boundary points are positive, you can't prescribe flowrate if you don't have water...

Generally speaking regarding to the tide, tidal wave is propagating along the coast at the scale of your model, so it's the gradient of surface elevation between north/south that is relevant, even on your east boundary. And your applying an homogeneous signal from the east, it's not really suitable.
Prescribing a sinusoidal signal at north/south can't work as it's not in agreement with your signal at the east (semi-diurnal with diurnal inequality).
You can first try to improve your model with the above comments and if it's still not appropriate maybe you should have a bigger domain and prescribing tide from other data sources, like a global database for instance (TPXO...)

Regards,
Laurent

Hi,

Thanks for all your comments, I really appreciate it.I'll reply to your comments in the same order you did it to me.

1. Actually, I copied the format from that section of that manual. I've checked one more time and I see the same things as in the manual. What is exactly the error in the format? Is it that they are not all aligned? I didn't have problems when running the simulation, at each time step, I could see the correct value of SL!

2. Yes, you are right with the boundary number, but I had the correct one in my simulation folder. I seems I just mixed them up when I copied to the folder I shared here.

3. I didn't want to prescribe the depth, but as you said, there is no watter there! So I had to prescribe also a depth. There is no water because I don't have section bathymetry for the river, so I decided to put the boundary there, as I don't mind what happens upstream. I had a lot of issues when generating the mesh, because of the shape of the boundary and the angle between both sides of the boundary.

4. According to my calculation, my prescribed sinus function has a 24 hours period, like my real signal at east boundary. I mean, there is no big difference between both values and I made the calculations so that they have, more or less, the same phase. Also, I understand that the value is prescribed at each node, the gradient in the boundary element is not so big.

I don't understand your comment regarding an homogeneous tide being prescribed on east boundary. Where or how do you think I should prescribe it, in order to be more consistent with the physics of the process?

Finally, I made the mesh again. I had to take out the river boundary and I'll place a source instead. At this moment, the simulation runs well with the closed boundaries. I don't like that option so much, because my boundaries are not far enough from my point of interest, but I couldn't make it work with the open boundaries. I still would be glad to you if you explain a little more about prescribing the tide on the east boundary, as I'm doing.


Best,
JR

Hi,

1- You have to write each couple of time and associated prescribed value of surface elevation on the same line. By copy/pasting from the user manual, you introduced line breaks which are not correct. If you look at the test cases, you'll see the right format of a liquid boundary file.
Your wrong file:
A correct file:

2- Bad luck...

3- You have to improve you mesh near the river. If you don't have any information about bathymetry and depth on this location and only flowrate value known, you can introduce some wet nodes locally on the boundary so as to prescribe the flowrate.
Introducing a source point instead is not exactly the same option, as a source point introduces momentum in every space direction, whereas a prescribed flowrate is perpendicular to the boundary, in the direction of the stream of the river.

4- Your real signal is not really a diurnal sinusoid... you have semi-dirunal inequality. The differences you're introducing with a perfect sinusoidal signal are likely to perturb your model on the boundaries.



Tidal current has to be generated by a free surface slope between the north and the south of your domain. But the signal you're introducing is the same from all your boundary points, so you have no free surface slope between north and south, it can be difficult to correctly reproduce the tide propagation with this method.
In the same way, side effects you're observing are created by the free surface slope in the west/east direction, where there is a discontinuity between your prescribed boundary (east) and your free boundary or land points (north/south).

Moreover if your point of interest is close to your boundary, I strongly advise you to build a bigger domain and to prescribe the tide from a global atlas. You can then check your model results with the signal you're currently using to prescribe surface elevation.

I hope it helps.

Regards,
Laurent

Thanks, I get your explanation now regarding the tide. As for the liquid boundary file, I think it's only your txt viewer, because mine shows it correct and when running, it shows the correct value at every time step.

I have one more concern related to the sources. You are supposed to prescribe the values for the velocities in the x and y direction. I tested with negative values and TELEMAC didn't tell me anything about the sign being incorrect, so I assumed that a cartesian system is used to include these velocities values.

Are you sure that the source adds the imposed discharge in every direction and doesn't take into account any sign included when prescribing the velocities? I couldn't understand how TELEMAC manages to prescribe a given velocity in all directions, and still comply with the x and y given components.


Thanks,
JR

Hi,

As you have the flowrate value for the river, I though it was easier for you to prescribe WATER DISCHARGE OF SOURCES (with no momentum addition, local velocities of the flow used), instead of velocities.
If you express this discharge as velocities, it depends of the local properties of your mesh. And cartesian momentum quantities are then added.

For this method, the source point should not be located on a liquid boundary point, but I think the previous solution of a boundary with prescribed flowrate is more suitable.

Regards,
Laurent

Hi,

I've taken into consideration some of your comments, but still I have no success with my model I really don't know what else to do to make it work!

I even changed to the wave equation because of its stability. I removed many dry cells because I was having salt at them, even when there had not been water there. So I left the shoreline as boundary, instead of having a full domain.

Below is a picture of my domain, now:


As you see, I also changed the orientation of the boundary, this one is aligned with the deepest contour level I have.

But the problem is that because of the closed north and south boundaries, I get reflection and those circulation patterns that should not be there. How can I do to get the north and south boundaries open? As soon as I try this option, even if I use thompson or not, it diverges.

I tried to use FV, as I'm more familiar with this method and maybe it's easier to treat boundaries, but not so many options are available when using FV and one of them seems to be the sources file. I realized what you told me about the source adding water in all directions and even when I'd prefer having the boundary there, I couldn't manage to make a good mesh when having the boundary at the river inflow in the lagoon, so I had to keep the source instead.

As you pointed out, I'm starting with zero elevation, but I'm trying to simulate 15 days prior to the time I want to simulate, in order to let the flow to be established and I thought it should work.

So, what else can I do? Or what I'm doing wrong? I just don't want to give up on TELEMAC! Please help me with some hint on what I might be doing wrong. This is some part of the Gulf of Mexico, by the way.

Best,
JR

Ps. I can't use a tide database because I added storm surge to my astronomical tide data. I add my steering file so that you can see the relevant options, in case you have a time to see it.

Hi,

I already gave you my opinion on your case.

For tidal process, I think that wall (222) or free (444) conditions for your north/south boundaries can't work and you have to prescribe something (544).
As you don't have spatial information of your tidal signal, you can try with the same signal as for your east boundary, but it can be instable aslo. You can try to adjust it so as to progressively reduce the free surface gradient close to land points. If side effects remain, you can try to introduce more diffusive processes on boundaries (increase the friction for instance), but it's not really a satisfactory solution.
A better solution should be to enlarge your model to prescribe tidal harmonic from a global atlas. It's also possible to add strom surge with this solution.

For you river, the best way is to prescribe the flowrate directly on the boundary (455), maybe with some local bathymetric corrections on boundary points to be wet.

FV scheme or wave equation options are not likely to change something here, it's your methodology which can be improve, not the model options.
I also strongly advice you to compare your model results with measurements (level and currents if possible).

Once your hydrodynamic model runs well, then you can introduce salinity and other features you have in your steering file (drogues). Tracer values can't appear on nodes where there is no water.

In a general way, you should increase the complexity of your model step by step instead of putting all the processes in your case at the same time, it's easier to understand your model behaviour.

Regards,
Laurent

Thank you for replying. Actually, that's how I started, step by step. But I'm running 6 different scenarios, so that means that even when I succesfully ran a test case, some of the scenarios don't behave the same than the test case. I ran the hydrodynamic model without tracers first, the only way was closing the boundaries and I got some results that (at the time) I considered they were more or less, correct. Because the tide and discharge conditions didn't force such circulation patterns, or at least, I couldn't see them (maybe because the velocities were very small, I couldn't see properly the direction of the velocity field at the sea). Also I ran for only 15 days, most of the problems start happening one month late, except when I run with north and south boundaries open (444), it fails almost right after starting the simulation.

Since I'm simulating 6 months, it would be hard to run 6 months only with Hydrodynamics, just for test and then do that for all the scenarios. As I said, getting correct results with one case doesn't mean I'll get succesful results with all of them. So I'd like to ask you a bit more about the options you mentioned.

1. If I'm to get tide from a database, which one should I use for being able to get also storm surge data, considering that I need information from year 1992 to date. And how long should I extend my computational domain from what I have now? At this moment, the deepest contour level is -17, located around 1.5km away from the shoreline.
2. If I decide to use the tide I have, with north and souht boundaries open, how long you think I should extend the east boundary so that the circulation patterns they generate, can't affect my area of interest?
3. The tide data that I have, was taken from a local database and it corresponds to a point located like 60 km away towards the south, but almost at the shoreline. I have checked that the tide varies just a few centimeters (2-4 cm) between the two stations I have around my area of interest. Being that said, do you think it would be acceptable to locate the east boundary in such a way that I don't have north and south boundaries? I'm interested in seeing the salinity transport inside the lagoon. And my first point of interest would be located like 500 meters or even a bit more, away from the boundary where the tide is being prescribed.
4. Might it work to set the north and south boundaries with V component of velocity null? (0 condition) or even both of them being 0? Then, the code for the boundary would be 400...is that equivalent to use high friction at the boundaries?

Finally I want to add that it's not that I simply don't want to extend my domain and follow your suggestions, it's that my tide data are supposed to be very accurate and it doesn't depend on me to decide to use another database. Although in such a extreme case, I'd have to. Another drawback is that I don't have bathymetry for the shallow region if I extend the domain, even when trying to use a database like GEBCO, they seemed not to have enough information for my area.

Thank you, one more time, for your useful comments.


Best,
JR

Hi,

1. From global tidal databases, you can only recompose the astronomical signal. Meteorological surges can be added from atmospheric data(bases), computed from sea level atmospheric pressure.
The extend of your model domain has to be in agreement with what you want to simulate: the propagation of tidal wave requires to correctly prescribe free surface slope.
For the surge, it depends on what you want to represent: spatial and/or temporal variations, or constant schematic surge.
Also the precision you need and the computational costs can be important criteria.

2. Once again, this solution isn't suitable. Because of your lake of informations, numerical instabilities enter your domain and propagate inside by intensifying. Model results are not correct, and the model can crash unexpectedly. You can try to add dissipative effects on boundaries, but it's not a satisfactory solution.

3. I'm not sure to really understand. Can you show a map with data you're speaking about? If you have 2 stations, the shift of few centimetres between them can be sufficient to represent the free surface slope. Maybe you can define your model boundaries on the stations locations...

4. I think this can't work also. I never tested this kind of tips for a real case, but I don't recommend it.

The accuracy of bathymetric data is also very important, and you need to have information in agreement with the resolution of your mesh.
This case is not an extreme one, it's rather classical.

Regards,
Laurent