open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi all!

I have a little problem.
I am modelling hydrodynamics in a network of canals with bridges and navigation locks and I have consequently defined a rather detailed mesh in some places with element size down to 1 m and with ca 70 000 elements in total.

I aim to model the whole system in 3D, but I start with 2D. This way I can see what is the time-step required to have Courant numbers below 1,0 and I can also use the 2D result file as a hotstart file for the 3D model.

Due to local high velocities, I need to have a time-step as low as 0,05 s in 2D (Courant number = 0,8), which means that even the 2D model requires rather long computational time.

If I use the same time-step in 3D with 10 vertical planes, then CPU time logically becomes huuuuuuuuuuuuuuge.
I am already running my case in parallel, unfortunately only on a "normal" desktop machine (4 to 8 cores), which means that I cannot really rely on parallel computing to speed up my case.

But am I not to violent to run my 3D case with the same time-step than in 2D? Can my model be stable with a larger time-step, and if yes, is there a method to assess roughly which value to adopt?

Another question related to this case: do other users have feedback on 2D continuations, especially on how long can it take to reach a steady state in 3D when starting from 2D results? I know it is highly case dependent, but as my 2D model reaches steady state after ca 5 hrs, it would be great if the 3D steady state could be reached significantly quicker than that...

Any help would be greatly appreciated!

Best regards,
PL

Hello,

Your time step really seems much too small, with a Courant number of 1 it would mean that you have elements of size 5 cm with a local velocity of 1 m/s, 5 cm this is very small for representing a network of canals. You can however have much larger Courant numbers (see e.g. the Wesel test case) and I can tell you if your steering file is optimum for this if you post it.
Typical comparison of computer times between Telemac-2D and 3D is a factor 4 or 5 it you have 2 planes.
Stability is about the same in 2D and 3D if there is no active tracers doing stratifications.
Note also that a very small time step is not more accurate, as convergence is obtained when time step AND mesh size tend to 0.

With best regards,

Jean-Michel Hervouet

Hello,

Thank you for your reply and explanations.

My minimum edge length is ca 0,3 m (around bridge piles). In these areas I have velocities in the range of ca 2-3 m/s, which means that with a time step of 0,05 s the Courant number should be of ca 0,3-0,5. I chose 0,05 s by running T2D with variable time step and a desired courant number of 0,8.

In 3D, should we only consider the horizontal edge lengths or does the vertical mesh size also influence the stability? I defined a very refined vertical mesh near the bottom (ZSTAR(1) = 0,01, ZSTAR(2) = 0,025 etc) to catch a logarithmic profile.
It means that in some areas the vertical mesh size between the lower planes might be of ca 5 cm.

I attach my steering files, both for T2D and T3D.

A last question: I defined two of the downstream BC as outflow by means of prescribed level and velocities, with constant velocity profile. The velocity was calculated by Q/A, with A = BC's width x (Zwater - Zbottom), with a constant bottom level. I don't excately obtain the desired discharge, and more strangely, the discharge is not exactely constant during the computation. This has been done only with T2D for now. I guess that one should not consider the whole BC's width to compute the discharge, but what is strange to me is that the outflow varies in time... Any tips on how to do it? I precise that the boundary option is 1, not 2 (Thompson).

Thank you in advance for your help!

Best regards
PL

Hello,

Generally the Courant number on the vertical is smaller than the Courant number on the horizontal and creates no problem (excepts in the case of settling velocity of sediments). When you refine on the bottom, keep in mind the grain size or Nikuradse coefficient. It is of no use to have a distance between the bottom and the next plane smaller than the grain size. Another point is that as soon as the first plane over the bottom is in the logarithmic profile and gives you the right U*, you get the correct stress, whatever the refinement. Last thing: this is valid if you use a Nikuradse friction law, which is not your case, so their is little interest in refining on the bottom.

Another thing: your scheme for advection of tracers is not mass-conservative, is it OK ? If not use scheme NERD (14).

On your downstream boundaries, it is an unsolved problem, if you prescribe both elevation and discharge, you do not solve the continuity equation, so there is an error of mass in the last row of elements. If you use the keyword CONTINUITY CORRECTION : YES, the program will give you the real discharge that obeys the continuity equation, and it may be different from the one you prescribe.

With best regards,

Jean-Michel Hervouet

Hi,

Thank you!

I use Strickler, but I refined my mesh near the bottom so that I can have a good repartition on the vertical for the results, since we are primarily interested in the near bottom velocities. Unfortunately we can't use Nikuradse law since coefficients needed for calibration doesn't match with the real bottom (mainly clays).

I don't have any tracers, so the advection scheme is not a problem (yet...). If we do sediment in 3D I will think of turning it to 14.

I will test with CONTINUITY CORRECTION = NO and see if the results are satisfaying near the boundary.

Finally, I made a test with a larger time step (0,5 s instead of 0,05), and the model is rather stable, at least in the areas of interest! So I will continue with that. Will even try it in 2D.


Best regards
PL