open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello,

I am currently running a coupled "telemac2d and sisyphe " simulation.

I am looking at alternate bars, in a 95m wide river, with à slope of 0.17%, using the MPM formula (Critical Shield value : 0.04 & D50 = 0.028m), at a constant discharge of 250m3/s, and a MORPHOLOGICAL FACTOR =6.

The model is running, but some oscillations appear in the river bed during runs (see enclosed PDF file).

I was wondering what could explain this (time step, mesh ... see below)

* is it linked to the time step ? the minimum edge length of triangles forming the mesh is 2.8m, as a consequenc I choose a time step of 0.8s to keep a CFL below 0.95 - (the velocity is around 3.5m/s)

* is it linked to the mesh ?

* could it be solved by adjusting to a really low (and unrealistic) value the "friction angle of sediment" ... in order ton keep a time step not to small ?

Before doing some tests on these several parameters, and in order to save time I would be glad to get your advices.

Thanks in advance for your help and tips.

Cheers !

Thibault

H Thibault,
could you make a figure with a small oscillating part of the model and with the grid and the bottom in order to see if the oscillations are formed by the grid?

I guess you have a regular grid with continues grid lines in flow direction. In that case you will always get oscillations (at least this is our experience at BAW). The only chance to avoid would be to create a new irregular mesh.
Try delauny triangulation instead of advancing front in your meshing software in order to get an irregular mesh.
Regards,
Rebekka

HI Rebekka,

Thanks for your quick answer... that's exactly that : I build my mesh so that I have grid lines aligned with the flow mean direction because my previous experiences with telemac2d (only - no sisphe) show me that calculations are faster when I did that.

I will try to change the grid, and to provide you with the figure you mentionned.

Best regards,

Thibault

Here are 2 figures with the MESH structure and the bottom oscillation.

You were right, oscillation are perfectly aligned with the mesh.

I will build another mesh with bluekenue, and try.

Thanks for your help,

Best regards,

Thibault

Hi Thibault,
that is exactly what we also see if we use this kind of regular grid. It is not a problem if you use hydrodynamics only. If you scale your color very fine then can you see velocity structures along the long grid lines even in hydrodynamics only. Coupled with morphodynamics there is a reinforcing effect and the problem increases and become not negligible anymore.
Good luck with a new grid!
Regards,
Rebekka

Hei,

Here are the results with the new grid unaligned with the main flow direction. Much less oscillation even if in one area there are still some cells aligned with the flow.

Just one more question, what tool do you used to create grid???

I use BlueKenue and I am quite happy with it, but in order to have an irregular grid I had to include some "random soft lines" because my model boundary is rectangular, so the grid was mainly aligned with the flow direction if i do not insert some perturbations.

Thanks for you help,

Cheers,

Thibault

Hello,

You could try to use gmsh, it's open source and free.
I am not sure if you would get a purely unstructured mesh with your very regular geometry but you can try.

You can use pputils scripts (search here on the forum for posts by Pat Prodanovic or search on github) to process your GIS-objects to inputs to gmsh as well as converting the gmsh mesh file to selafin.

Good luck!

Best regards
PL

Hello,

thanks for the tips, i will look at this,

Best regards,

Thibault