open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi all,

I am trying with coupled Telemac-2d and Sisyphe (v6.0 - g95 - Windows XP) to simulate a classical case of a steady flow in a 90° curve (see mesh and project attached) so that I could throw the effects of the secundary currents on the sediment transport into relief.

There should be sedimentation in the inner side of the curve and erosion in the outer side, and then "meanderings".

I have a canal 30cm wide making the curve, steady flow 8L/s, water depth 6.6 cm, grain diameter 1 mm.

I encountered two problems:

-I cannot ask for a very long DURATION as I am stuck with a very small time step (automatically around 10^-2 second) resulting in a res data of great size (for example DURATION = 3 hours then result = 8 gigas). If I ask for a bigger one (time step or courant number) it wouldn't converge after a while.

-I can't get a steady flow, as perturbations keep appearing. I have a steady inflow and a water surface level at the outflow, I tried Thompson as well. I checked my water level at the outflow it should be good.

As a consequence I don't become the result I should. I know this is not a difficult simulation, I have a lack of experience.

I would greatly appreciate any help/piece of advice!

With best regards,
Jean

Hi
Your problem with the result size should be solved by changing the output periodicity (it's 1 by default) but you could say 100 and obtain a result every 1s. You also divide by 100 the size of your result.
Search for graphic printout period in the keyword.

For the bed evolution, take care of the sedimentological upstream boundary condition to avoid false local bottom evolution that could also generate free surface oscilation.
With a water depth of only 6.6 cm, small changes could generate great consequences.
It's also possible that some clipping could occur or that precision should be increase
Hope this helps

Hello,

I cannot open your curve.rar file here, maybe the parameter file only would be sufficient, but anyway you should start with hydrodynamics only. Your small time step is due to the fact that you reproduce a small physical model, but is however strange. Why "automatically around 10^-2 second" ? Do you try a finite volume option ? Then move to finite elements, with wave equation option, and see what kind of time step is reasonable. For the dataset of results, use the GRAPHIC PRINTOUT PERIOD. There is no need of Thompson method in such a case. Be also aware that in a physical model, the values of diffusion coefficients currently used, like e.g. 0.1 m2/s, are far too large.

With best regards,

Jean-Michel Hervouet

Hello,
I could not open your rar file but I'd recommend the following:
1) try to get a steady state hydrodynamics simulation (only Telemac)
2) use this solution as hot start of a Telemac+Sisyphe simulation
3) As JMH mentioned in the previous response, I don't see the point to use a Thompson BC.

Important -> Take a look to the validation tests.

All the best,

Pablo

Dear Jean,
finally I was able to open your files. I'd like to stress your attention to the following :

1) For the numerical parameters (hydrodynamics solution) you can try :
TYPE OF ADVECTION = 1;5
SUPG OPTION = 2;2
TREATMENT OF THE LINEAR SYSTEM = 2
SOLVER = 1
SOLVER OPTION = 3
IMPLICITATION FOR DEPTH = 0.6
IMPLICITATION FOR VELOCITY = 0.6
MASS-LUMPING ON H = 1.
H CLIPPING = NO
SOLVER ACCURACY = 1.E-6

with a smaller time step (0.1s could be a good choice)

2) For the sediment transport/bed evolution coupling, be careful with the
COUPLING PERIOD.

I hope this helps,

All the best,

Pablo

Hello,

Alternatively you can use :

SUPG OPTION = 0;0
COMPATIBILITY OF FREE SURFACE GRADIENT : 0.9

This is the other way to avoid the spurious oscillations due to the so called inf-sup condition (i.e. possible spurious solutions when depth and velocity are discretised in the same way).

With best regards,

Jean-Michel Hervouet

Dear Christophe, Jean-Michel and Pablo,

Thank you so much to all three for your answers!

The flow is now steady and works well, I use the result as start condition for the coupled calculation with sisyphe.

I took your advice into account,

-result file is of fitted size thanks to adapted print out period

-Jean-Michel, sorry for not being clear I meant "automatically" for the time step as I used the VARIABLE TIME STEP option. The thing is the "ill-posed problem" appeared each time I had tried a bigger one so I ended up using the option. I always used St Venant EF.

-Thank you Jean-Michel and Pablo for the keywords. Wave propagation and conjugate gradient for the solver improved the steadiness a lot. Could you please explain briefly in which way they contribute to stabilize the calculation? Does it work for bigger models too?

Thanks again!

Cheers,
Jean

Hello Jean,

Actually in the wave equation the velocity is eliminated from the continuity equation, to get the depth. There is theoretically two differences with the primitive equations:

1) there must be mass-lumping of mass-matrix for velocity.
2) divergence of gradient) is really Laplacian in primitive equations, it is the diffusion matrix in wave equation (this is a reason for more stability, because this slight mistake will in fact smooth instabilities).

BUT, in version 6.1, there is an implicitation on depth that is set to 1 in wave equation (line TETAC = 1.D0 in lecdon_telemac2d.f), this may be also a reason why it is more stable. This will be removed in version 6.2, to enable more accurate computations of tsunamis.

The conjugate gradient has nothing to see with stability. It is just that with wave equation the matrix of the linear system to be solved is symmetric. With primitive equations it is not (and the system is much larger because it couples depth and velocity). In this latter case solvers like GMRES or normal equation must be used.

The message "ill-posed problem" occurs when you have at the exit velocities that enter the domain. It may happen with von Karman eddies or after a bend. It is just a warning, but sometimes these entering velocity may grow to infinity (they are free, so it is still a solution of Saint-Venant equations). Unless you see strange recirculations on the exit or crashes, you can discard the message.

With best regards,

Jean-Michel Hervouet

Hi all

Here are some small comments on numerical parameters given by Pablo

For the following Keywords
TYPE OF ADVECTION = 1;5
SUPG OPTION = 2;2
H CLIPPING = NO
Those values are the default value so it's not necessary to add them in the sterring file.

The Keyword SOLVER OPTION is used only when SOLVER = 7.

Hi Jean,

Regarding your second question: the correction is independent of the size of the model. For further details, you can take a look to the classical reference of Walters R.A. and Carey G.F "Analysis of spurious oscillations modes for the shallow water and NS equations", Computers and Fluids 11 (1983)2: 51-68.

All the best,

Pablo