open TELEMAC-MASCARET The mathematically superior suite of solvers

Hi!

I need to model the influence of a floating pier. I thought of two methods for doing it:
- with porosity with Telemac-2D
- with Telemac-3D by modifying the near surface veleocity field at the pier location (UVW = 0).

I think Telemac-3D would give somewhat more accurate results. But I am just wondering how can we change the near surface velocity field? Can it be done and if yes, in which subroutine(s)? My idea is to have let's say one or two plans under the water surface that are fixed a certain elevations on which I could set velocities to 0 to model the pier.

Thank you in advance for your help!

Regards
PL

Hello,

A clean solution would consist of adding head losses where the pier is. This can be done in subroutine source.f

Example :

SL1U%TYPR='Q'
SL1V%TYPR='Q'
SL1W%TYPR='Q'
CALL OS('X=0 ',X=SL1U)
CALL OS('X=0 ',X=SL1V)
CALL OS('X=0 ',X=SL1W)
N=356
XNORM=SQRT(U%R(N)**2+V%R(N)**2+W%R(N)**2)
SL1U%R(N)=0.5D0*XNORM
SL1V%R(N)=0.5D0*XNORM
SL1W%R(N)=0.5D0*XNORM

will add a headloss to point N=356. You can inspire from what is done for vertical structures to get an idea of which values to put on.

Then it could be that a local atmospheric pressure would do the weight of the pier...

With best regards,

Jean-Michel Hervouet

Thank you.

A few questions: do you really mean "SL1U%TYPR"? I only find "S1U%TYPR" in either source.f or declarations_telemac3d.f.
Just to make sure: is this source term applied only at free surface?
When you mention vertical structures, do you mean dragfo in Telemac-2D or is there a similar function in Telemac-3D?
Finally, if I apply a local atmospheric pressure, will this add some local head losses or should it be done either way in source.f?

Thank you in advance!
PL

Hello,

Sorry, it is of course S1U and the like... S1V, S1W : implicit source terms, note that they are added at the left-hand side of equations, thus positive for a head loss.

Yes dragfo gives an idea of the headloss values.
The atmopheric pressure will not add headloss, it wil just act as a body weighing on the free surface.

Regards,

JMH

Hi!

I just made some first tests on a (too much) simplified flume geometry, and I have some questions regarding the best way to model velocities near the surface in case of wind.

The model is rather short, 20 m and 3 m deep. Wind is 10 m/s in X direction.

Velocities in a longitudinal section are given in graphs below for different turbulence settings. The flow at surface goes from left to right, and opposite direction on the bottom.

1/ UV: Smagorinski, W: Mixing Lengh Quetin (5)



2/ UV: Smagorinski, W: Mixing Lengh Tsanis (6)



3/ UVW: Smagorinski



3/ UVW: k-epsilon




First, we can see that the channel is not long enough to obtain a steady state, especially for k-epsilon. Nevertheless the model gives interesting results allowing to make a quick comparison between different turbulence models.

The two first tests seem to give rather good results. Near the surface, Tsanis model gives higher velocities than Quetin.

Smagorinski on UVW gives rather good results in depth but the gradient near the surface is much higher with maximal velocities ca 2 times higher than with Tsanis.

The test with k-epsilon is hard to comment since the model is obviously too short for turbulence to develop. But it seems to give a smoother velocity profile along the vertical, with a somewhat lower velocity at the surface (ca 60 % the velocity obtained with Tsanis).

Initially I was planning to use either UV : Samgoringski + W : Mixing Length (5 or 6, models adapted for wind driven currents) or k-epsilon. It seems that velocities at the surface can differ rather significantly between these two types of models. Should k-epsilon be avoided in case of wind driven currents?

Finally, a last word to say that the above results integrate a source term on the water surface to account for head losses due to floating pier (without local pressure though), but the computed drag coefficient (0,05 * UNORM) is too small to have a significant effect (the is enhanced by the fact the surface velocities are also rather small). But the implementation with an artificial higher value (0,5 * UNORM) showed good results.

Thanks in advance for any tips :)

Regards
PL

Hello,

With k-epsilon we use the stress due to wind at the free surface to plug it into the k equation, instead of computing the gradient of velocities (which depends on mesh refinement near the free surface), the effect is that we get a better level of turbulence at the free surface, so I would rather trust the k-epsilon model. Other models seem to have the velocity at the free surface rather disconnected from the rest of the domain, due to a lack of turbulent diffusion.

You also should be careful with vertical cross sections and look at horizontal depth averaged velocities. Even in 2D the steady state solution that we would expect with Saint-Venant equations (wind stress balanced by free surface slope) is not seen because horizontal recirculations break the symmetry, and in 3D it may be even more complex. So if you move your cross sections along the y axis you may see different solutions.

Regards,

JMH

Hello,

Thank you Jean-Michel for these useful explanations on k-epsilon.

I now made some new tests to include the weight of the piers by adding 0,5 m pressure head on their location. Unfortunately I don't manage to obtain satisfaying results.

The test I made include only the extra pressure, without wind nor drag term, with Smagorinski on UV and ML on W (I will try with k-epsilon now...).

Velocity UVW



Velocity U



Velocity V



Velocity W




We can see that the water surface gradient near the pier induces high velocities in the model, which are not realistic compared to what I want to model... Apart from the velocity values I also don't reach a steady state.
I made some tests on certain parameters to see if they can play a role, but I always obtained a similar flow field. The parameters tested so far are:
- hydrostatic / non-hydrostatic
- small time step (down to 0,05 s)
- surface gradient compatibility down to 0,0
- implicitation coefficients to 1,0
- with/without filter for hydrostatic inconsistency
- advection scheme for velocities : 14

As my model only has solid boundaries, a certain part of the instabilities might indeed be wave reflections due to the application of the extra pressure at fist time step. I tried to apply it progressively with a time ramp and still got the same results, even after a long simulation time.

I know that such a method had been previously applied (if I remember right it was used to model the water surface under a ship for a lock model - but I can't remember where I saw it...). In that case I assume that the velocities at the surface "under the ship" were ca 0 to have a stable state.

Do you have any recommendations to obtain more realistic results?

Thank you a lot in advance !

Best regards
PL

Hello,

I have no experience, maybe you should smooth a bit the shape of the hydrostatic pressure, otherwise we create a large pressure gradient at the boundaries of the pier ? (but this should be compensated by the free surface).

One thing to try could be :

DYNAMIC PRESSURE IN WAVE EQUATION : YES

I'll try (but not soon...) a test with a boat in a basin to see if you arrive at a steady state.

Regards,

JMH

Hi Jean-Michel!

I tried with DYNAMIC PRESSURE IN WAVE EQUATION : YES and k-epsilon. I have a stable model but still with high velocities induced by the pressure gradient.

I did not try yet to smooth the gradient on the edges. Will try.

I attach an image of the results with the mesh. Maybe a very refined mesh at the interface would work better? The nodes on which I apply the extra pressure are located within the red area.





Thank you in advance!

Regards,
PL

Hi!

Last update. Including a smoother pressure gradient on the two neighbooring lines of nodes (outer pressure boundary) did not help.

The only way to reduce velocities in that region, with my case, has been to use constant velocity for U and V. After a few tests, it seems that U and V tend to zero if velocity diffusivity tends to infinity.
The last test I ran was with 100 m2/s, but then the model crashed due to instabilities...

There might some other tests to perform, but it starts to be beyond my skills / scope.

So for now I will only use a drag force in source term to model the piers. I am however of course curious to see if you can manage to reach a steady state with the water surface under a boat...

Thanks for your help.

Regards,
PL