open TELEMAC-MASCARET The mathematically superior suite of solvers

Dear Telemac users,

New to the Telemac tools, I am trying to model a wastewater discharge (point source with fixed flow rate) on a simple coastal 2d mesh taking into accounts local currents (open boundaries with fixed UV).
My simulation is running but the results (enclosed) show inconsistencies in water elevation values..
Boundary conditions velocities also do not seem to propagate in the domain.
Any ideas of the reasons of these behaviors?
Should you have advice on the proper parameters for this kind of modelling/or links towards similar works, please do not hesitate!
Thank you,

Thomas

ps: parameters files enclosed

Hello,

When using TELEMAC, it is recommended to use a plane projection (e.g. Lambert or UTM) rather than longitude/latitude. You seem to model the Bay of Frejus, do not you? In that case, you can use Lambert 93, Lambert 3 South or UTM 32.
Maybe redo the mesh/geometry file.

Anyway, you cannot prescribe only velocity along the liquid boundaries and should at least prescribe water level somewhere along them.

Your model seems simple, but you can also model tide in your area with TELEMAC. You can have a look at the TELEMAC-2D tide example and use the local solution Mediterranean Sea for the database of tidal constituents. The options used may help you defining the steering file.

Some comments about your steering file:
- CORIOLIS COEFFICIENT is not used if not setting CORIOLIS = YES,
- if modelling scalars/tracers, you should use a conservative advection scheme at least for this variable, such as PSI or N if you do not have tidal flats (your case) or better the last advection schemes available: in your case, I would recommend TYPE OF ADVECTION = 5;5;5;5 with SCHEME OPTION FOR ADVECTION OF VELOCITIES = 2 and SCHEME OPTION FOR ADVECTION OF TRACERS = 2 (if you do not have tidal flats, your case, = 4 otherwise). These are the same advice given by my colleague Agnes for TELEMAC-3D,
- try first OPTION FOR LIQUID BOUNDARIES = 1 (classical, rather than Thompson) and check at the boundaries that it is prescribed what you expect,
- SOLVER ACCURACY is quite big, you should perhaps decrease it to have accurate results when the results start to be better,
- SOLVER OPTION is not used if not setting SOLVER = 7,
- if not using any specific TURBULENCE MODEL, you do not need to write MAXIMUM NUMBER OF ITERATIONS FOR K AND EPSILON information,
- you do not need to write STEERING FILE in your steering file, in particular if the name is different from what is written inside.

Hope this helps,

Chi-Tuan

Hi Chi-Tuan,

Thanks a lot for your help, I might come back to you latter on when my model will get more complex, but for now everything is running fine.

Thomas

Hi again,

I am facing now new interrogations when switching to telemac 3D on my above case.

I have a liquid boundary with prescribed H = 0 on the sea side and a closed solid boundary on the land side.

I have wind influence from the north.

1. The UV velocities and Tracer (enclosed) in the 2D result behave completely differently compared to the Telemac2D run. Can you think of a reason?

2. Also in the 3D results I see my tracer at the bottom layer (enclosed) (source elevation is on the bottom) but i can barely see it coming up at the top layer (enclosed). The tracer is freshwater outflowing in seawater and hence should come up quickly. How can I implement this difference in salinity/density?

3. Finally my goal is to simulate propagation of suspended sediments, sediments deposit on the bottom, and propagation of bacterial pollution. Apparently all those tasks can be performed on Telemac 3D, do you confirm?

Steering file and results enclosed.

Thanks a lot.

Thomas

Hello Thomas,

Which version do you use? V8P0?

2: you should use tracer/scalar with name 'SALINITY G/L ' (please read the User Manual, in particular for the number of characters for the name and unit of tracer/scalar, when using WAQTEL, it may prevent you from errors) + DENSITY LAW = 2 or 3 (dependent on salinity or salinity+temperature) to take into account buoyancy effects as active tracer/scalar, or even = 4.

3: yes, TELEMAC-3D can be coupled with WAQTEL for water quality processes and SISYPHE or the new GAIA module for sediment transport processes.

Comments on your T3D steering file:
- ABSCISSAE OF SOURCES + ORDINATES OF SOURCES: if your source is located on a mesh node, you can use the keyword GLOBAL NUMBERS OF SOURCE NODES,
- forget the keywords ACCURACY FOR VERTICAL VELOCITY, MAXIMUM NUMBER OF ITERATIONS FOR VERTICAL VELOCITY (or even SOLVER FOR VERTICAL VELOCITY, PRECONDITIONING FOR VERTICAL VELOCITY) as they are not used by TELEMAC-3D (they have been deleted in the trunk),
- if using LAW OF BOTTOM FRICTION different from 0 (no friction), you should define the keyword FRICTION COEFFICIENT FOR THE BOTTOM,
- your keywords "ACCURACY FOR..." = 1.E-4 should be decreased if you want accurate computations, in particular for tracers/scalars,
- do not write the keyword STEERING FILE in particular if it is different from the name of the file, it can create problems,
- you should define a VERTICAL TURBULENCE MODEL, by default it is constant viscosity and in real cases, it does not often give good results.

Anyway, as told in other topics of TELEMAC-3D, you should read the recommendations written by my colleague Agnes : www.opentelemac.org/index.php/kunena/21-...se-with-some-figures
In particular for the SCHEME FOR ADVECTION... = 5 + SCHEME OPTION FOR ADVECTION... = 4 which are less diffusive than 14 or 13 for SCHEME FOR ADVECTION...

To conclude, after setting better parameters, you may have to refine your mesh close to the source.

Hope this helps,

Chi-Tuan

Hi,

Thanks a lot.

1.I curently use V7p2.
Shall I switch to V8P0 for the functionnalities I want to use?

2. Concerning Salinity I don't get how to input the difference in salinity between my input and the receiving waters?

3. For the schemes of advection, I am not able to use 5. Actually when I change parameters I often get errors "MURD3D:ITERATION NO. REACHED 100 ,STOP" or "TRID3D subroutine: Preconditioning 17 impossible".
From what I read in the forum it seems like my mesh contains tidal flats? I wonder why, that should not be the case?
I also get huge velocities close to the shore.. (enclosed)?

Best regards,

Thomas