[i2a]

Hello Everybody,

Background: Object fully immersed (single phase) in water and falling under gravity. I am using the 6DOF solver (properties for which, are defined using a UDF as usual) in FLUENT.

Question: Do I have to explicity apply the buoyant force in the 6DOF properties UDF e.g prop[SDOF_LOAD_F_Y] = 100 N. I can easily get a number - because the body is fully immersed.

My Understanding: As far as I can understand the 6DOF solver should take care of Buoyancy automatically. As, in certain cases (object falling under gravity from air to water), the situation can get quite complicated and may require an interesting UDF for Buoyant Force calculation, which will be far from elegant for the multiphase users. Moreover if am not mistaken buoyancy is just the force due to the pressure difference between the upper and lower faces of the body (thinking of a square). As we are solving for pressure in FLUENT it (Buoyancy) should be automatically accounted for by the 6DOF solver.

Reason for the Thread: I think (do not have any experimental number) my object is falling with somewhat higher velocity. Hence the question.

Thanks very much,
Awaiting.

[sergoblin]

Hy,

I'm also simulating argon bubbles rising in liquid tin at constant temperature (500K) and constant atmospheric pressure. I do it in Fluent with VOF scheme. I also include surface tension and wetting angle on the wall between argon and tin. This model is very simple so it should not be any problems: after some time bubbles should rise to the surface because of densities difference ( buoyancy force against gravity force ). But it does not happen (the bubbles sink to the bottom of the tube and stay there till the end of the simulation) so I understood that here buoyancy force is somehow neglected... I would really appreciate if someone help with that issue!

[sergoblin]

Hy,

I'm also simulating argon bubbles rising in liquid tin at constant temperature (500K) and constant atmospheric pressure. I do it in Fluent with VOF scheme. I also include surface tension and wetting angle on the wall between argon and tin. This model is very simple so it should not be any problems: after some time bubbles should rise to the surface because of densities difference ( buoyancy force against gravity force ). But it does not happen (the bubbles sink to the bottom of the tube and stay there till the end of the simulation) so I understood that here buoyancy force is somehow neglected... I would really appreciate if someone help with that issue!

[hrvig]

Hi,
We have been struggling with the free fall motion of a flat plate in water.
We did some simulations by letting the plate fall freely parallel to the direction of gravity and monitored the position as function of time (using the motion history option provided with the 6dof solver).

The results show that a plate parallel to the gravity direction fall at almost 9.8 m/s^2 , suggesting that buoyancy is not included.

We then applied a external force using prop[SDOF_LOAD_F_Y] corresponding to the buoyancy and found the results to be reasonable.

If you have any question, please let me know.

Best regards,
Jakob

[danielfc]

I am facing the same problems you guys mentioned above.

Now I am curious. In my setup it also seems like FLUENT ignores the buoyancy force and it has to be "artificially" included. But in this case, is the fluid force not calculated considering fluid pressure integration? Does the software remove the hydrostatic contribution? Whats is the reason for that? Stability?

I have also a more practical question. In my case, there is a spring connected to the body inside water, but the movement is not being damped as I expected. Any guess why?

By the way, I read your Master thesis Jakob. Nice job!

[hrvig]

Hello danielfc,

Yes, when Fluent does the integration, the hydrostatic contribution is not included :-) You can however easily add it using a udf:

#include "udf.h"
DEFINE_SDOF_PROPERTIES(dof_udf, prop, dt, time, dtime)
{
prop[SDOF_MASS] = mass of object here
prop[SDOF_IZZ] = moment of inertia around z axis here
prop[SDOF_LOAD_F_Y] = total buoyancy force here
}

I think it is left out automatically, when the models you have selected do not require it.

I have never modelled a spring connected to a body but could the buoyancy force explain it?

Thanks for the comment on my Master thesis. However, there are plenty of things I would have done differently today :-) Isn't always like that?

Enjoy the 6DOF modelling,
Jakob

[danielfc]

Hi Jakob,

I saw how to do it in your thesis' appendix! It is not my case right now, but I was just wondering how tricky it could be if you have a body with wetted volume changing during the simulation like a ship in waves, for example.

If the buoyancy effect is included or not is just a matter of the maximum amplitude, but my problem is that the amplitude is not being reduced by the fluid damping as I expected.

[hrvig]

If you do such a simulation (ship in waves) using the VOF I am sure there is an easy way to do it. I guess it is already implemented as density differences are already specified when you setup the case.

How well do you resolve the flow around your object? Could that explain the difference?

[danielfc]

Well, regarding the buoyancy, I think you are right and I will explore that.

With respect to the flow around the object, I am working with a simplified mesh and therefore I don't expect high accuracy results, but it should promote anyway some degree of damping. The results until now have shown either steady or amplified movement, what is physically meaningless. I am working on a even more simplified model in 2D in order to find out what is wrong in my setup.

[danielfc]

Having a hard time with this issue.

The 2D model has the same behavior.

Does anyone has experience with mass-spring system in FLUENT?

The time evolution of the mass vertical coordinate is attached.

[samir_cfd]

Hi Jakob
I am simulating the 6 dof falling ball in water using Fluent but I have a problem, when the ball is close to the free surface the solution diverege (divergence problem) I don't know where is the problem exactly and how to solve it?
Many thanks!!

[RJE]

i'm modelling a spring in fluent and i don't know how to do to model K and the preload. I'm using ansys for the first time, can anyone help me ?

[vinerm]

Fluent has an in-built spring model. You just need to provide stiffness and preload.

[RJE]

i thought that i have to model a new material using udf to model the spring wich is attached to a solid in one way and fixed from the other side.
am i in the right way ?

[vinerm]

Even if Fluent did not have a model for spring, creating a material would not be a way; that would be a process in structural simulation but not in Fluids. In CFD, it just has to be the equation governing the force due to spring.

[RJE]

hi,
so let's say i have F=F0+K *dep ; and of course we know K and the preload how can i attach this equation to the solid in fluent ?
u have any idea ?

[vinerm]

You do not need to attach any equation. When it is said that a model exists within a tool, it implies the mathematical model, i.e., equation is already included. All it requires from the user are the parameters, stiffness and preload, if any. These values need to be entered within Six-DOF Properties Dialogue Box.