open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello!

I've to simulate a flood in a river. So I want to impose a constant flow on the upstream. I've still impose a water depth and a velocity in the initial conditions. The problem is that when I impose a constant flow in fudaa, the simulation doesn't work.

I tried to change the conlim file to impose a flow and a waterdepth upstream and it almost worked. The problem is that the requested flow is never reached. (The upstream flow is 2.2m3/s when I asked 3m3/s). So how can I do to impose an accurate flow upstream?

The second problem I encountered is that the results seem roughly correct with a time step of one second but the water levels are crazy when the time step is 10 seconds. Do you know where does this problem come from?

Thanks for any answer!
Penic

Hello,

First thing, Fudaa just helps you to fill the parameter file, you can bypass it and edit this file directly, and run the program without Fudaa, but your problems seems to come from the fact that you impose the depth at the entrance in a fluvial flow. You must relax the depth (4 5 5 in the boundary conditions file), but an important thing is the initial conditions, you must have water at boundaries where you impose a discharge.
As you probably also impose the depth or elevation at the exit, you will not see the correct discharge at the exit in the listing unless you use :

CONTINUITY CORRECTION : YES

in the parameter file (because the equation h = imposed depth replaces the continuity equation, and we need to take care of that).

I hope this helps,

Jean-Michel Hervouet

Hello JMH!

Thanks for your quick answer! Telemac works(with the restrictions I wrote in my previous post) when I impose the flow AND the water depth ( 5 5 5 in the boundary conditions file) but it doesn't work when I only impose the inflow (4 5 5 in the boundary conditions file). Note that I also impose the water depth downstream and that CONTINUITY CORRECTION : YES was still written in the parameter file!

Hello,

So it must be another mistake, nearly all fluvial cases work with the condition 4 5 5 at the entrance, unless your case is supercritical at the entrance, in which case you are right to impose the depth also, then the problem of getting the correct flux becomes tricky, still for the problem that we then do not solve the continuity equation at the entrance. I realise that in this case the CONTINUITY CORRECTION = YES is maybe not the thing to do, so you can also try to remove it.

Regards,

JMH

Hello,

I come to you because I still have not solved my problem of flow.

So I imposed a flow and a water depth upstream (5 5 5 in the conlim file). I modified some Fortran files to obtain the hydrograph at the end of the simulation. Do you know why Telemac can not impose the speed required of him?

Regards
Baptiste





(The txt file is in reality a .liq file)

Hello,

This is an open problem and a paradox, when you impose the depth at the entrance, the continuity is not solved (it is replaced by the equation depth=prescribed value), so you get the requested depth and velocity, but the discharge is not correctly transmitted by the first row of elements. When we have a free depth, the continuity is solved and we can get exactly what we want. This explains the small differences that you have and this is why we prefer subcritical boundaries.

Regards,

JMH

Tanks for your answer! You said that I get the requested depth and velocity. But I didnt impose any velocity. So with which velocity does TELEMAC make its calculations?

Baptiste

Hello,

With 5 5 5 in the boundary conditions file, you impose a discharge and the program will assume a velocity with constant module and direction perpendicular to the boundary (the module will be deduced from your prescribed discharge). There are other options (velocity proportional to the square root of the depth for example) but the default is constant.

Regards,

JMH

Ok, but to deduce the velocity, telemac divides the flow by the area isn't it? In which case, I don't understand why the flow upstream is not the flow I imposed.

Regards

Baptiste

Hello,

If you use CONTINUITY CORRECTION = YES, the discharge computed at the entrance is not deduced from the values at the entrance but from the continuity equation, so differences are observed but the value printed is really what is entered into the domain. If you use CONTINUITY CORRECTION = NO this is more surprising, but the depth that contributes to the flow is the one that is in the divergence term of the continuity equation : div(hu), which is generally taken at time n or, with sub-iterations, is based on the implicitation of depth. If I remember well it is programmed so that the discharge takes into account a linear variation between depths at time n and n+1.

Regards,

JMH