open TELEMAC-MASCARET The mathematically superior suite of solvers

Good afternoon

I am modelling sedimentation in a reservoir, using 2D telemac couple with GAIA. Because of the characteristics of the sediment, I am only considering suspended transport of cohesive sediment (plus an initial sand bed in the whole domain for bed stability).

When the water level of the reservoir is high, most of my elements are wet and the reservoir in fact reaches the upstream boundary. Nevertheless when the level starts to fall, the condition near the upstream boundary changes to a "free flowing river" that reaches the reservoir now located lower in the mesh. My problem is that in the elements that change from wet to dry, an excessive and unfeasible sedimentation takes place (more than 50 m).

For the steering files I used the recommended values for tidal flats that both the telemac and the gaia manual provide (I attached the files), nevetheless I still can not solve this problem.

I was wondering if there is another recommended configuration or Keyword that can help reduce the excesive sedimentation problem.

Thank you very much in advance.

Kind regards,
Eduardo

Hello Eduardo,

I cannot understand if the hydrodynamic behavior is what you expected: is the model working well without sediments?
Indeed my first suggestion would be to check the hydrodynamic as first step. About parameters, I can see that you use a variable time step for finite elements: I would use a constant (and smaller than 200s) time step. For SCHEME FOR ADVECTION OF VELOCITIES, I would also suggest to change to 13 or 14 (as for tracers).
When you will be satisfied with hydrodynamic, then I would add sediments to the model.
About parameters in Gaia, as you already set low values for CLASSES CRITICAL SHEAR STRESS FOR MUD DEPOSITION, I have no particular hints for the high sedimentation.
Maybe some of my colleagues with more experience in sediment modelling have some ideas.

Best regards,
Sara

Hello Eduardo,
Please find below a couple of fast hints to test.
(1) For cohesive sediments, I don't suggest using values of settling velocities computed by Gaia. Try to provide explicitly a value.
(2) Try a very high value for CLASSES CRITICAL SHEAR STRESS FOR MUD DEPOSITION (=1000 for example), meaning that you'll have deposition all time, just to see how the system behaves.
(3) your time step is perhaps a bit too high...
Hope it helps,
Cheers,
Pablo

Good afternoon Sara and Pablo,

Thank you very much for your reply.

I changed the scheme for advection of velocities to 14 and imposed the settling velocities (0.001 m/s for a sediment diameter of 0.00001 m) , but I still have the problems. Actually I modified the starting point of my mesh (moved downstream on my river) to try to avoid the most problematic tidal flats areas (not all can be avoided), but it did not work.

I tested just the hydrodynamic part and it is working fine, no problem with the tidal flats on my domain, but when I couple it with gaia, now my sediment deposit directly in my boundary condition (see figure below).

I do not understand why this happen, because even though the velocities are low (2 cm/s) the settling velocities are even lower in magnitude (1 mm/s) for which the sediment shouldnt deposit directly in the boundary. I also used the keyword TREATMENT OF FLUXES AT THE BOUNDARIES=2 as suggested in the forum to avoid depositions near my boundaries, but it is not working.


I highly appreciate any suggestions.

P.D: With respect to one of the previous suggestiosn, I am using a variable time step because I am simulating a 3 year period, and as part of the project the simulation have to be run multiple times (stochastical calibration) so reducing the computational time is extremely important. So I what that the time step is small when my inflows are high but as big as possible (but still stable) when my inflows are low. I imposed a desired courant of 0.5 to make is as stable as possible.

Hello Eduardo,

Have you solved your problem? Cause I think we have the same question! Excessive deposition and erosion will happen at tidal flats area. I am confused now and do not have a good solution yet.

Hi Shan!

I never fully solved the problem but I did reduce the sedimentation enough to make the model fully functional.

I saw from your other post that you are working with telemac 3D. With respect to 3D I found something in this post, maybe you can try it out www.opentelemac.org/index.php/assistance...f-cohesive-sediments

All the following advice are for 2d, so I do not know if they apply to your case, but nevertheless, you can check them out.

I found two possible explanations for the unphysical sedimentation.

1. You can check one in this forum post, but basically, it says that the unphysical sedimentation is due to an overestimation of velocities when we have an element with wet and dry nodes, and we use the finite element method ( www.openmascaret.org/index.php/assistanc...sisyphe?limitstart=0).

2. The second possibility was explained to me by Ms.Rebekka Kopmann (she is a moderator in other telemac forums). I attach her detailed explanation in a pdf below, you can read it there.

3. With respect to the fully unstructured mesh that Ms Kopmann suggested, I used gmsh with a Delaunay triangulation (inside gmsh go to Tools- Option - Mesh - General and change the meshing algorithm to Delaunay that is fully unstructured), maybe you can try that one.

4. Also, in the sedimentation is in the boundary condition directly use VELOCITY PROFILES = 1 and TREATMENT OF FLUXES AT THE BOUNDARIES=2.

I attach the steering files that gave me quite decent results, you can check them out. Again, they are for a 2D case so I do not which commands are still valid for 3d.

Hope this helps!

Kind regards,
Eduardo