open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello everyone,

we setup a 2d model of a large reservoir which was running very stable and lead to promising results even with sediment transport (t2d_advection_1.JPG).
However, the switch to telemac3d led to problems that we have not yet been able to solve.
Consequently, I have reduced the complexity and I am currently simulating steady-state hydrodynamic conditions only.
I have tested a coarse and a refined mesh. The model has tidal flats (very shallow areas) and deep areas (water depth > 55 m). In the last tests we used 5 vertical layers (PRISM).
Since we were not able to get a stable 3d model, we tested several schemes and observed the following :

- Method of characteristics (1) worked ok for the finer mesh but there are fluctuating and non plausible velocities close to the tidal flats in shallow areas (see t3d_advection_1.JPG).

- Explicit MURD scheme (14) leads to an exceeding of the maximum iterations in some timesteps and very bad results t3d_advection_14.JPG.

- LIPS scheme (5 for advection and 4 option for advection) leads to non plausible results after very few timesteps (very similiar to 14).
However, there are no error messages or exceeded maximum iterations.

We also tested the 2D continuation and experienced that an unstable model setup will remain unstable (which makes sense).
I'm not sure if we did some mistakes in the steering file or if the problem is mesh related?
Do you have some recommendations or other things we could test? Please find some of the steering files enclosed.

From my experience with the SSIIMM 3d code, I recall that setting a minimum water depth to create the first cell was the most effective way to stabilize the model.
Do you think that those flat cells (5 cells even in shallow areas) cause the problems?

I appreciate any advice or ideas.

Kind regards,

Kilian

Hello Kilian,

If you have not succeeded in solving your issue, here are some ideas to try:
- change the VERTICAL TURBULENCE MODEL, e.g. to mixing length (VERTICAL TURBULENCE MODEL = 2) + MIXING LENGTH MODEL = 3 for example. Except to get analytical solution, it is not usual to use the default constant viscosity over the vertical,
- you can try set IMPLICITATION FOR DEPTH and IMPLICITATION FOR VELOCITIES to 0.9 + decrease FREE SURFACE GRADIENT COMPATIBILITY down to 0. but I am not sure this change your current results a lot,
- try to decrease the time step if the Courant number is too big,
- try a coarser mesh and see if the issue still occurs. What about the size of elements in the center of your domain but also in shallow water areas?
- what about the type of the open boundaries? Are they all with prescribed flowrates? (code 4 5 5)? Or is there at least one boundary with a prescribed elevation. If all with the same type of boundary, the problem is ill-posed.

Hope this helps,

Chi-Tuan

Hello Chi-Tuan,

Sorry for my late answer. I had quite a long winter break.
Thanks for your ideas they all slightly improved the results.
In any case, some questions arose:

- Actually I used 455 for all open boundaries and set additionally an initial water level. Is this necessarily ill-posed? After I read your suggestion I set 555 for one of the inflows but there were no big changes. The outflow is through a turbine and I thought also about just prescribing the water level at the outflow open boundary. However, few mm of water level change would lead to immense volume changes since it's a large reservoir which is why preferred to define the discharge directly.

- The main problem are the rather high velocities close to the tidal flats (neighboring nodes have water depth 0) which cannot be physically explained because the main flow is in the centre and looks reasonable. I realized that the height of the cells in those areas (e.g. sidearms) is much smaller than in x and y direction and the growth rate might be critical in some cases. So probably the mesh quality is not good enough in those areas and causes instabilities? Is there a recommendation to avoid those rather high velocities (only compared to the very low velocities in the reservoir) next at tidal flats?

Best,

Kilian

Hello Kilian,

Refining your mesh may be a good idea, you should try if not already done.
Try to avoid flat triangles, obtus angles and too big ratio of sizes between one triangle and its neighboors (a few percent only, times 2 is not good e.g.).

Hope this helps,

Chi-Tuan