open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi all!

I have a model that I have been using to simulate thermal dispersion. It has worked fine so far. No I need to include stratification with salt. The new results show erroneous currents within zones where my mesh is refined (I must refine the mesh here to model piles), see the attached pictures. Earlier results with only temperature were OK.

My mesh has the following characteristics:
- horizontal spacing: 0,5 m in the detailed zone, up to 50 m elsewhere
- vertical spacing: only horizontal levels (MESH TRANSFORMATION = 3) with dz = 1 m and 21 planes.

I use k-epsilon but also checked with Smagorinsky and Mixing length on the vertical, similar results.

I use the hydrostatic version as the non-hydrostatic is far to costly (the model runs on a commercial HPC...).

I tried to lower my time step but without noticeable improvements.

I also attach my steering file.

Does anyone hve faced similar problem? Can this be fixed by tuning some numerical parameter?

Finally, I have a question about the keyword AVERAGE WATER DENSITY. In subroutine dssurr.f it is mentioned that it should correspond to density for water temperature 15 degree and salt concentration of 0 g/l but such information is not present in documentation. Can anyone confirm that this value should be defined according the information in subroutine dssurr.f?

Thank you in advance for your help!

Best regads
PL

Hello Pierre Louis

You need to explain a bit more your problem, with only these pictures I can not understand the problem. You are showing only Temperature without and with salt?

Waiting for more details, hereafter 2 remarks
1- it is well known in the 3D community that the nonhydrostatic version is much more efficient that the hydrostatic one. Yes it is more expensive, but you should run it at least once to see the improvement that will induce for your case
2- the refined areas are two close to the boundaries that you didn't refine in the same way. This causes a high element growth ratio which causes numerical issues including high diffusion. It is worth to resample boundaries in the same way than the refined areas

I hope that this helps

with my kind regards

Riadh

Hello Riadh!

Sorry for not being so clear. Here comes some more explanations.

I want to model the outflow from a heat power plant. In a first round it was made without any stratification - just a simple thermal dispersion with a different temperature in the outflow compared with the sea temperature. I then need to include salt stratification (in the sea water and with a different salt concentration in the outflow).

The two first pictures show the 3D velocities with a model with only temperature while the second corresponds to the case with both temperature and salt. In that case I observe what I called "erroneous currents", that is wriggles on velocities (also observed on the tracers) in the areas where my mesh is refined (and especially at the transitions between refined and coarser mesh).

Regarding non-hydrostatic, of course, I normally use this version for all my 3D models but on this one in particular it is simply not possible from a budget point of view (!). But I might rethink the whole thing by removing the detailed outlet geometry (node spacing 0.1 m in some locations in combination with the highest velocities of about 1 m/s) to retrieve a more reasonable set-up.

And since I am going to rethink it all I will take your advices regarding element growth ratio near boundaries into account, thanks!

A last comment. The outflow has actually a non-negligible air concentration that messes up the actual fluid density which is of utmost importance in this case. I have just worked on a trick in order to account for air concentration and deaeration effects on the flow density by doing the following:
- adding a third tracer playing the role of air "AIR" (volumic concentration)
- introducing a decay rate for this tracer to model the deaeration process (very simplistic, constant decay over the water column)
- correcting the fluid density in subroutine drsurr.f with RHO = RHO*(1-AIR)

It works fine on a small test model but (of course) crashes in my big model Has anyone tried to do a similar thing and if yes, any comments/advices? I will continue to work on it since I must include the deaeration effect on fluid density to obtain a proper calibration.

Best regards
Pierre-Louis

Hello,

Yes an hydrostatic assumption with buoyancy gives wrong results, see e.g. the mixing of two fluids in my book, even with small velocities where you would expect a hydrostatic hypotheses to be true. This is observed with other software so it seems to be mathematics rather than a numerical effect due to a specific algorithm.

The average water density is really the average water density in your model, in the sense that the approximation 1/(RO+DELTARO) = 1/RO (1-DELTARO/RO) requires DELTARO to be as small as possible, so the average RO is really 0.5(ROMIN+ROMAX) in your domain.

With best regards,

Jean-Michel Hervouet

Thank you for this information.

I will give feedback here on how it goes with the new set-up once I have som results.

Best regards
PL

Hello,

I just wanted to give a quick feedback here. Using the non-hydrostatic version have sorted the problem out.
I did also managed to implement a fictive tracer with decay to model air contained in the water and its deareation process. Results were in good agreement with measurements!

Best regards
PL