open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi,

I am trying to calibrate the modelled velocity profile at a location from my regional model according to some reference data but struggled at seeing any improvements (and changes) by varying different parameters. It would be grateful if one can advise on what I can change on the configuration.

For the profile shape, please see the attached figure.

I am using slip boundary condition at the bottom, with 10 horizontal layers (8 out of 10 was fixed) and Nikuradse law with a uniform ks = 0.075. Horizontal and vertical turbulence model are smagorinski and mixing length respectively. There are several things that I have tried but still failed to see any significant changes on the profile shape:

1. Varying roughness size ks:
I have tried to run the model with ks (m) = 0.03, 0.05, 0.08, or even a non-sensible value of 0.2.

2. Varying vertical and horizontal diffusion coefficient:
For horizontal, I have tried values of 1.E-4 and 1.E-6 (default). For vertical, I have tried 1.E-6 and 1.E-8. However, I noticed that the vertical diffusion coefficient contributes very little to NUZ when I was checking (effective) viscosity at the bottom layer in x and z direction (see figure attached - NUZ is significantly larger than NUX), so I decided to play with the vertical turbulence model as well.

3. Vertical mixing length model:
Changing the model from Prandtl to Nezu and Nakagawa. Switch off damping function (by setting to 0).

Playing with these parameters and models did not give apparent changes to the streamwise velocity profile shapes. I have not yet played with k-eps model but I am hesitant to do this due to large aspect ratio of my regional model in certain areas. I also wonder if the 2nd layer (1st layer above seabed) placement is important to the results as well, as it seems like there is a dominant factor that I have not yet realised.

Thanks you so much for your patience! It would be grateful to hear your advice.


Best,
Ray

Hello Ray,

It would be interesting to upload one of your steering file + Fortran files + one figure of the extent of the area + location.

Do you know how your reference data are built? From measurements? Average during a period of time? How wind is taken into account for this reference? Can you use wind data as input for your model?

Anyway, my first idea would be to try the k-epsilon model and see how it behaves for your configuration. It is not always easy to tune mixing length model over the vertical.

Chi-Tuan

Hi Chi-Tuan,

Thanks so much for your reply.

My regional model domain is roughly 200km x 160km large and the specific location that I am interested in is refined with roughly 3m cell size (see attached figure). Reference data to tune from is field measurements so that it was averaged over a time period for a specific flow speed and the abnormal velocities near free surface (first 10-20% of the water column) can be neglected. Water depth around that location is between 40 to 50m but it can go above 100m at wider region.

I have tried the k-epsilon model on both horizontal and vertical. The steering files and fortran file are attached. It seems like the agreement of the velocity profile is better on flood than ebb tide (see figures). And the sensitivity of ebb velocity profile is so low - no matter what models and configurations I used, there is still big discrepancies at the lower half of the water column.

With many thanks,
Ray

Hello Ray,

Can you try to find a power function z = a.U^b which fits the better to your curves (measurements + computations / flood + ebb)?

Looking at your steering file, I wonder why you have chosen some values for keywords and not the default values:
- BYPASS VOID VOLUMES = YES
- TREATMENT ON TIDAL FLATS FOR K-EPSILON = 0
- MINOR CONSTITUENTS INFERENCE = YES
- CONTINUITY CORRECTION ON OPEN BOUNDARIES = YES
- FRICTION COEFFICIENT FOR THE BOTTOM = 0.05
- LAW OF FRICTION ON LATERAL BOUNDARIES = 5
- VERTICAL VELOCITY DERIVATIVES = 2
- HYDROSTATIC INCONSISTENCY FILTER = YES
- MAXIMUM NUMBER OF ITERATIONS FOR ADVECTION SCHEMES = 3500 (above 50 or 100, you should wonder if the time step is OK or if there is a specific issue with what you have built).
- SOLVER FOR PROPAGATION = 2

I do not think the results would change a lot but I am surprised by a few choices.

If you use conjugate gradient as a solver (= 1), you can use corresponding preconditioning equal to 34 (= 2 * 17) which is a combo of 2 preconditionings suited for conjugate gradient, the efficiency of this method is to be improved in term of CPU time. e.g. for PPE in your case and diffusion of velocities.

You can try IMPLICITATION FOR DEPTH with a value different from 1 (0.99 or less for example but not 1).

Anyway, you can play with the mesh distribution, e.g. use MESH TRANSFORMATION = 2 with a logarithmic distribution, increase the number of planes... As you do not model stratified flow, using Z layer mesh transformation is not mandatory.

Hope this helps,

Chi-Tuan