open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi all,

I am running into perplexing issues with an idealized version of a more complex case that has its own issues. Essentially, I have a straight channel with a bottom slope of 0.005 m/m and lateral slope of 2:1, of 50 m in length. I have estimated a certain downstream depth (about 0.25 m) based on Manning's roughness and a given inflow. In theory, the flow should be subcritical everywhere.

The problem is that within the first 60 to 90 seconds of the simulation, certain apparently random nodes on the inlet boundary suddenly give a depth < 0.001 m and the Froude number shoots way up (I've seen values > 20000), crashing what should be a subcritical boundary. The strange thing is that these nodes are not in the shallow part of the boundary, they are at what should be the deepest part. Moreover, the immediate neighbours of these nodes are all at the expected depth (0.25 m to 0.30 m), creating a very steep gradient.

I've tried making the boundary narrower, and I've tried different solvers, sets of equations, time steps (fixed and variable), initial conditions, velocity profiles, etc as listed in comments in my .cas file (see attached for .cas, .cli and .slf). I've also tried finer meshes than this one (this one is at 100 mm distance between adjacent nodes) which have the same problem. The problem is the same in serial and parallel, and appears to occur with both single and double precision selafin files.

I could try setting an upstream depth, but this seems to me like a band-aid on a deeper issue.
(I should mention that flow is from right to left, on account of the laboratory setup this parallels.)

Does anyone have any idea what could possibly be going on and leading to this numerical instability? I could hardly conceive of a simpler scenario than this one, and yet it cannot "get off the ground" compared to more complex models I've tried!

Thank you in advance,
André Renault

have you tried with an inital water level at the same elevation as you boundary condition and a discharge increasing from 0 to 0.72 m3/s?

It seems like you 'shock' the model.

Hope that helps,
Patrick

Another thing you can do is extend the model upstream and create a deeper section. I think part of your problem are the bank slopes of your model, with an extension upstream you can make all boundary points the sema depth/elevation.
Patrick

Hi Patrick,

Your answer in #42312 seems to have worked! I wasn't really thinking of having an inflow hydrograph to increase discharge progressively, but it worked. I increased inflow by 0.1 m3/s every minute and this seems to have been "gentle" enough to work. Thank you for the suggestion, I will keep this in mind in the future!

Kind regards,
André Renault

Hi all,

I spoke too soon... I have different issues now! The upstream boundary segments are really strange; it seems as if all of the discharge is pouring through one node adjacent to the right edge of the boundary, causing a very high velocity and depth. In addition, the depth is near zero on the rest of the boundary, and then ripples up and down in the inlet node before stabilizing. The instability only increases with time.
At one point, I tried narrowing the boundary to restrict it to nodes that should remain wet, but this only moved the weird node inward.

The figures below are of water depth and free surface, but the velocity values follow the same pattern. For context, I'm expecting a uniform depth of about 0.25 m but have a strange spike of 2-3 m at the boundary node and have near-0 depth on the boundary itself.
Early time steps have a more or less even inflow, before merging into the second-from-right node.

*there's supposed to be another figure here but the forum is deleting it*


What could possibly be causing all the flow to slosh through 1 node? Maybe the fact that flow is from right to left (this doesn't seem likely)?

I have attached my newest simulation files, please let me know if anything is missing. As documented above, I have tried varying many parameters: solvers, depths, velocity profiles, roughness, mesh size, and so on.

@Patrick: Thanks for the deep section suggestion. What length and depth would you suggest, and how should I transition from a flat bottom to a trapezoidal section without causing detrimental instabilities?

Thanks,
André Renault

Well, I'll answer my own question here and say that I should've tried this long ago, but refused to out of principle, thinking there shouldn't be any supercritical flow.
I set the upstream BC as Q+H instead of just Q (5 5 5 instead of 4 5 5), added an upstream depth corresponding roughly to what normal depth should be for this Manning's n, and it seems to have practically solved the issue. I need to do a bit more research to make sure this is the case and my boundary widths still need adjusting, but so far so good...
So if you are stuck with a supercritical depth on entry, do try adding a fixed depth even if you think it should be subcritical!

Hello André,

Indeed, if you have a supercritical flow (you can visualise Froude number with VARIABLES FOR GRAPHIC PRINTOUTS including F), the theory tells that 3 informations are need at the inlet in 2D (thus 2 components of velocities/flowrates + water level).

Chi-Tuan