open TELEMAC-MASCARET The mathematically superior suite of solvers

Dear All,

I am attaching a simple test case file in which I am simulating flow in a channel. I want to use the non-hydrostatic option but when I turn this on simulation gets stuck after 3 seconds.

Everything runs smoothly if I use the hydrostatic version, I was wondering if there is something special that I need to care about while using the non-hydrostatic version.

Attached is my case file. Also could somebody comment on usually what are the tings that I need to be careful about if I want to use k-e turbulence model.

All help is greatly appreciated.

Kind regards,
Sumit

Hello,

Here are a few hints on your parameter file :

/ This is very small! it should work with a larger time step unless you have a scale model
TIME STEP = 0.01

/ This is useless unless you do non linear waves, remove it
NUMBER OF SUB ITERATIONS FOR NON LINEARITIES = 2

/ no use of GMRES here, diffusion system is symmetric, put 1 instead
SOLVER FOR DIFFUSION OF VELOCITIES = 7

/ you can try implicitations of 1., much more stable
IMPLICITATION FOR DEPTH = 0.6
IMPLICITATION FOR VELOCITIES = 0.6

/ with constant diffusion the coefficient should be larger, e.g. 0.1 or 1 (if not a scale model...))
HORIZONTAL TURBULENCE MODEL = 1
COEFFICIENT FOR HORIZONTAL DIFFUSION OF VELOCITIES = 1.E-6

/ try at least mixing-length on the vertical (option 2)
VERTICAL TURBULENCE MODEL = 1
COEFFICIENT FOR VERTICAL DIFFUSION OF VELOCITIES = 1.E-6


/ you can go down to 0 to stabilise
FREE SURFACE GRADIENT COMPATIBILITY = 0.9

/ has very little effect, put NO
CONSISTENT PROJECTION = YES


Once it works you can try the k-epsilon model, but with large elements (which is often the case in free surface flows), I always wonder what is the meaning of the velocity gradients found by the program and feeded to the k-epsilon model, they must be too low and the model must give too small diffusion. What you must be careful with is boundary conditions of k and epsilon. Sometimes the domain is such that the turbulence has no time to establish and then you only see in your model what you have given at the entrance.

With best regards,

Jean-Michel Hervouet

Thanks a ton JMH.

Results have certainly improved, specifying horizontal turbulence as 1 with coefficient as 0.1 did the trick in vertical I am using turbulence model 2

I am still having problem with non-hydrostatic version, it just hangs after some time.

By the way PPE is only solved for non-hydrostatic version right? So would it help if I change preconditioning for PPE. Maybe I should continue computation from the converged result of the hydrostatic version while using the non-hydrostatic model.

Thanks once agin.

Kind regards,
Sumit

Hello,

Normally preconditioning 34 (i.e. diagonal + direct solution on the vertical) is good for PPE, but 2 (only diagonal) should do it as well. It would be good to know what happens (in what step the program is stopped... probably in the characteristics because of diverging velocities somewhere ?).

Regards,

JMH