[mojtabaivi]

hey there.
I'm beginner in Flow3D an I have some question about that:
1) Do I need to define reference pressure (1atm) or It is defined in default?
2) I think the blank space of model is filled with air? is it true? or not?
Thanks

[JBurnham]

Blank space is called 'void'. It has constant pressure, and does not undergo gas-law dynamics. In other words, treat it as ventilated, zero-velocity. Navier-Stokes equations are only solved for the liquid, not in the empty void.

If you turn on physics > bubbles > adiabatic bubble then the void gets ideal-gas law pressure/volume (pressure decreases when void region expands, increases when void region gets smaller), but still does not have Navier-Stokes momentum, so no velocity. Thermal bubbles (volume also depends on temperature) are also possible.

If you use two-fluid model option, then there are two fluids (liquid and gas) and no more 'void'. Then the gas phase includes velocity, momentum, pressure, etc.

So you have a lot of choices.

[mojtabaivi]

Thanks a lot. So what is the best choice for modeling an air-entraining vortex?

[JBurnham]

Laminar flow or LES turbulence model. RANS turbulence models like k-e RNG and standard k-e assume isotropic turbulence (turbulent fluctuations in x, y, and z are all the same strength), and will therefore damp out vortices.

My best suggestion is to model the vortex without any additional physics besides gravity and LES turbulence (or laminar flow) until you have a good solid vortex core. Then if you want to add air entrainment you can, but wait until you have a fully functioning vortex core model before adding advanced physics.

You will probably need cell resolution on the order of 1 to 2 cm or finer in order for this to work, though it depends on the size of the vortex. Make sure your boundary conditions are far enough from the vortex that they don't interfere with the vortex formation.

If you have a valid license then you have access to the FLOW-3D Users Site: there are several vortex simulations that can be downloaded from there. Check those out, they will explain a lot to you.

[spf521]

Do you have a valid license? I want to find a one to download some simulation examples. Thanks!

[mojtabaivi]

Thank you for the time spending for me.
So physics are: gravity and Large Eddy Simulation turbulence.
Can you tell me what is the best boundary condition for this case?
inlet:specified pressure-fluid elevation
outlet (which is a submerged cylinder pipe): specified velocity (Froude number is usually above 1) - volume flow rate that is going out is better but unfortunately the software do not accept negative amounts of flow rate (but why??!)
top face is symmetry and others are wall
are these OK?

Thank you very very much

[JBurnham]

You can make a negative flow-rate boundary by setting Volumetric Flow Rate with positive Flow Rate magnitude, and then set the flow vector to point out of the domain. For example, if the Vfr boundary is on z-min, then set the z flow vector to -1 to point down. Make sense?

Keep in mind that when you use a Vfr (flow rate) boundary, it turns into a velocity boundary where each cell has the same velocity. That means that if your boundary removes fluid by way of an outward-pointing vector, that boundary must be submerged 100% or it won't pull out the correct amount of fluid (there will be blank air cells on top with velocity not removing fluid).

Everything else looks okay, as long as the pressure boundary is far enough away from the vortex that it doesn't interfere with the vortex formation. Maybe 4x the flow depth is far enough?

Good luck!

[mojtabaivi]

I employed all your tips, but no vortex was appeared! I've really got confused.
anyway, Thank you very much ,dear Jeff. I learned many things from you.