open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello!

I have a flat water depth despite changing my drag coefficient, even at unrealistically high numbers. I'm not sure how this could happen? Given the above it makes me wonder if it's a numerical issue and/or something to do with my *.cas file. I've had successful runs with previous data-sets of the same channel so I know the free surface is not what's expected; the topographic differences are very small.

Testing the simulation there are no changes despite altering the advection scheme, the mesh edge length, xyz point density, and generally tweaking the *.cas file.
I've tried different mesh densities also.

One of the changes I've made is the keywords:
NUMBER OF CORRECTIONS OF DISTRIBUTIVE SCHEMES = 1
NUMBER OF SUB-STEPS OF DISTRIBUTIVE SCHEMES = 2

Could this impact it?

Many thanks!

Hello,

We have recently corrected a bug, but only in the trunk, that was cancelling explicit source terms for the predictor-corrector options (scheme option... = 2 or 3). You can try scheme option... = 1 of advection schemes 4 and 5 (N and PSI) to be sure that it is not your case. Or take murd3d.f from the trunk in library telemac3d and put it in your Fortran file.

With best regards,

Jean-Michel Hervouet

Hello,

Thanks for the reply.

My free surface is now fine - it was in part due to convergence issue. The free surface now seems to adjust with changes to the CD coefficient. However, despite prescribing head losses at various layers on the bottom I now get odd, really high TKE values along the boundary. I had previously rectified this by prescribing head losses at the first four bottom layers of the mesh. I imagine this is related to the bug cancelling out the constants applied to each layer?

Using a new mesh I also seem to be getting huge mesh contortions at the inlet of my river. There's little topographic difference between the meshes (as mentioned above.) What in particular about a mesh can cause such changes? I've seen some small contortions before but nothing this bad.

With kind regards.

Hello!

Comparing my results for the same steering file and fortran file (and thus same drag) for v7p1r1 and v7p2r3, I've noticed that I get odd TKE values even when using a non predictor-corrector scheme (advection scheme option 14), and that my streamwise velocities measure much higher.

The difference in the velocity profiles make me think it's a continuity issue. What is troublesome is that v7p2r3 recognises the code to set my first four layers but doesn't seem to attribute the roughness values. Hence I now get high TKE values again at the bottom boundary.

Despite getting good results with v7p1r1 I want to use an advection scheme that's second order (e.g. PSI) and compatible with wetting and drying (new scehem option for predictor correcto), hence why I want to use v7p2r3. However when using scheme option = 4 the same issue is still present, so it may not be due to the predictor-corrector bug.

Is there a major difference between the two versions which could account for this? It's left me scratching my head.

Hello,

Maybe you should change the boundary conditions for k and epsilon (in cosake.f if I remember well, or in kepscl3.f to see the actual implementation). By default we choose conditions on derivatives dk/dn and d(epsilon)/dn because we think of wind, but in simpler cases Dirichlet values are more sensible.

I am also surprised by the very small time step. You could try to have a larger time step.

With best regards,

Jean-Michel Hervouet

Hello,

I was restricted to a small time-step as i got the "exceeding max iterations" error for anything above 0.1. However, by changing the Solvers to option 7 and the Preconditioning to option 2 I now get a nice run with a much larger range of time-steps and with little-to-no spurious spikes at the inlet (as seen above). It works well with the option 5, the PSI advection scheme, but it seems to crash with the "exceeding max iterations" error when testing it with option 14.

Are their specific Solvers which cannot be used with option 14 etc.?

Thank-you for the advice on the boundary conditions. I'll look into it.

Bets regards

Also, my free surface no longer changes with drag again. The main thing I've changed has been the solver and pre-conditioning. The solution converges fine so it's not the issue I had previously...

Solved it! Mostly an issue with the mix of solver's I've been using. It now runs without error and with the expected results.

In one of my older steering files I specify VERTICAL TURBULENCE MODEL as K-Epsilon, and then go on to state MIXING LENGTH MODEL = 3. From what I remember Telemac uses the last option specified. Am I right in assuming that the vertical turbulence is solved using the mixing length model in that case?