Learning Forum

[Joël Danton]

[Nilay Pedram]

Hello,
Can you please describe your question?

[Joël Danton]

Hello,

During my intership in a marine biodiversity company I have to simulate a small strucutre under waves close to the coast. The aime is to use CFD to help dimensionning the strucutre by extracting forces in play due to waves on the structure. Following the theory, my structure is forced by Drag and Inertia (Morrison equation). Therfore, my question is, which software of ansys should I use to obtain what I need ? Ansys Fluent with open multiphase flow and open wave BC condition OR Aqwa ?

(I have been using Ansys Fluent multiphase... for the last month and now that I'm finally having some results, it seams that I cannot obtain inertia force.)

Thank you for your help

Joël

[Rob]

Is the object floating or fixed? What exactly do you need to know? 

[Joël Danton]

The object is fixed and under water. I need to extract the horizontal and vertical forces induced by the waves on the structure. 

[Rob]

Fluent. Monitor the force components in the Reports. How far under water is it?

 

[Joël Danton]

I'm working in multiphase flow with open channel and open wave BC with F.S. set at 3.7m and Bottom level at 1.4m (So water height is 2.3m right ?). My body is of Ø1.2m x 2m high and is place on the bottom. The wave is 4th order stokes with H=0.58m and Lwave=16m.

[Rob]

Check the depth/height specification. I think it's linked to the mesh position, so whilst the height is 2.3m (you're possibly correct) based on the numbers given I don't know the mesh coordinates. 

Check the mesh resolution around the top of the unit and free surface, you may find it'll break the surface and needs a higher cell count in that region. 

[Joël Danton]

Concerning the forces results: The  horizontal forces are accurate enough compare to results obtained by an other software, but not for the verticale forces. Indeed if we focuse only on the bottom surface, when I ask for the lift force on this face in the report definition, the results is pretty big (~20000N). Thus, when I try to exctract only the force induce by static pressure (density*g*depth), by using EXPRESSION "AeraAve(StaticPressure,[bottomBC])*Surf.[m^2]" the plot shows almost the same results (~20000N), which  lets believe that the vertical force is induced mainly by the static pressure. When plotting the dynamic pressure (1/2*density*velocity^2) by the same way (EXPRESSION "AeraAve(StaticPressure,[bottomBC])*Surf.[m^2]"), it appears that the force is very low (~100N). Though, what was expected is that the dynamic pressure should induces at least a force oscillation of +/- 1000 N around 0 N. Do you know how could I easily plot this force induced by dynamic force only and that is maybe more correct than what I did ?

[Rob]

Lift Force or Force Report? Remember anything using velocity in an equation on/adjacent to the surface will be influenced by the fact the wall is at zero velocity. 

[Joël Danton]

I need the vertical force induced by the wave velocity on a plate. As particle trajectory of a wave is orbital, velocity is arriving frontaly and ajdacently to the surface of the bottom-plate. The issue is in the choice of the force in Ansys Fluent. Indeed, neither lift or vertical force report seams to correspond to the orbital movement of the velocity of the wave.

[Rob]

Are you checking the force on just that plate (single face) or over the whole unit? How well resolved is the near wall mesh? Ie what y+ values are you seeing over a wave cycle?

[Joël Danton]

I'm checking the force on just the plate (single face). The plate is Ø1.2m and has a surface of approximately 0.94m^2. The mesh cell size is about 0.03m. For y+, see picture.

[Rob]

That's not ideal, but shouldn't cause too much of an error. However, it does suggest you've not reached the equilibrium state and you may need to run a few more waves. Have you set the operating density to that of the water?

[Joël Danton]

Okay, i will do that. It is a transient simulation. I don't really set the operating density. But it is set up as minimum-phase-avereged. Should it be changed ?

[Rob]

Set to zero. It shouldn't make any difference to the solution but may help with the reports if you need to correct for hydrostatic pressure as that's then rho_l.g.h  

[Joël Danton]

I tried. I'm not sure it has worked.
Concerning the convergence of a transient simulation, how do you define that it has converged or not ?

Secondely, here is the plot of the vertical force on the bottom plate. My goal would be to configure a plot of the vertical force with the same oscillation but oscillating around 0N. It would be kind of a relative vertical force. Do you have a idea how can it be done ?

[Rob]

For a transient there's the time step convergence (ie does each step converge) and have the monitors reached any form of repeating pattern. The latter may be much more difficult if there are several transient effects with different frequencies, and some cases never exhibit a perodic result. 

Re the above, if you correct to the mean force does that give a sensible answer? I suspect you've got a hydrostatic effect in addition to any slamming forces. We (staff) are also limited in what level of input we can provide - ie it's limited to what's in the manuals and "public knowledge". 

 

[Joël Danton]

Ok. Yes if the mean force is postpone to 0N, it would give a sensible answer. I understand, thank you for the help and time already given.