open TELEMAC-MASCARET The mathematically superior suite of solvers

Hello everyone,

I'm working on a study of a wastewater flume in the sea water.
I would like to set the water temperature accordingly to some data we have.
The thing is, the temperature of my study area is changing rapidly with the depth (23 on the surface-19 at 40m depth).
I tried to initialize the sea temperature with CONDIM and then to force the boundary condition with BOR3D. But it's not working well. In fact, I can't get the stratifiaction/layers I'm lookling forward. After the first time step, the temeprature is homogenizing.

Do you have any advice in order to make this work ?
Or maybe it's not feasible ?

You'll find attached my fortran file (the modifications are stressed with the keyword MODIF).

Best regards,

Hello,

There are possibly several key points to keep stratifications stable:

1) horizontal planes. There is an example in condim.f
2) filtering hydrostatic inconsistencies
3) k-epsilon model

I also enclose a parameter file (in French) of our Berre lake study, which has stratifications, with temperature and salinity.

With best regards,

Jean-Michel Hervouet

Hello Jean-Michel,

Thank you very much for your answer. I tried the three options you adviced me (as you can see on the case file and fortran file attached). But I still don't get a stable stratification (pictures).






I think I'm missing something regarding the boundaries. I'm not sure of my depth test at the boundary points.

IF(ITRAC.EQ.1) THEN
IPOINBOR2 = NBOR2%I(K)
IPOINBOR3=NPOIN2*(NP-1)+IPOINBOR2
IF(MESH3D%Z%R(IPOINBOR3).GT.-10.D0) THEN
TABORL%ADR(1)%P%R(IBORD)=23.D0

Is that correct ?

With best regards,
Rémi

Hello,

I just see DENSITY LAW : 0 in your steering file ? Shouldn't it be a law that takes the temperature into account ?

11 planes was a minimum for the Berre lake, and my colleagues use now 32 planes.

Otherwise your implementation of bord3d.f seems correct, provided that the tracers are imposed at this border (beware that sometimes mesh generators put 2 for tracers even on liquid boundaries...).

With best regards,

Jean-Michel Hervouet

Jean-Michel,

You are right I forgot to set the DENSITY LAW to 3...

So I run another simulation with that law and an increased number of layers: 30.


The results are better but I've noticed that the water is getting colder nearshore and then it "spreads" all over the domain.
So, now I'm simulated a case without wind as advice by Alexander.
I'll keep you inform.

Thank you very much for your time,
Regards,
Rémi

Hello Rémi,

Strong wind
WIND VELOCITY ALONG X=20

can also be a reason. Especially without density stratification
DENSITY LAW= 0

Best regards
Alexander

Hello,

As expected, it works much better with a density law=3 and a moderate wind. Thank you again

The boundaries of my domain correspond to prescribed depth and velocities (566). I've prescribed a 0-velocity on the parameter file, so I get some issues regarding the vectors (high values of vertical and horizontal components).




So, I tried to change it with a 544 condition. But the velocities are even worst (unstable), even with a Thomson condition

How should I parameterize my boundaries?
During the simulations I've made so far, I get the message:
GRACJ BIEF : exceeding maximum iterations 100
What does it mean ?

With best regards,
Rémi

>So, I tried to change it with a 544 condition. But the velocities are even worst (unstable), even with a Thomson condition

>How should I parameterize my boundaries?

Could you check that LITBOR is also 4 in order to avoid density gradient along the open boundary?

5 4 4 0.000 0.000 0.000 0.000 4 0.000 0.000 0.000 389 4 # openBoundary (14 - 27533)
5 4 4 0.000 0.000 0.000 0.000 4 0.000 0.000 0.000 624 5 # openBoundary (14 - 27533)

Hello,

You are now in the general problem of open boundaries, which is partly unsolved in 3D. For the Thompson boundary conditions, I am not sure it works with wind, the depth averaged velocity has no real meaning in this case. If the velocity is free, the main problem is spurious velocities when the flow enters the domain (the problem is then not well posed). In our Berre lake study it was solved by adding a very small head loss at the boundary points (enclosed subroutine source.f in file princi.f). In this case the geometry allowed a simple implementation based on the coordinates.
If you prescribe a velocity equal to 0 it may trigger problems because the only degree of freedom for a divergence free field is the vertical velocity. The best would be to prescribe measured velocities.

With best regards,

JMH

Hello Jean-Michel, Alexander,

I solved my problem using the head loss method.
Thank you for your precious advices !

you 'll find attached the results of a simulation. The wastewater, which is hotter and less salty than the deep sea water, is gettint up in the water column before spreading in the surface layers (hotter).
And the temperature and salinity gradients create important velocities.




Best regards,
Rémi