[armlic]

Hello everyone,

I´m trying to complete the parameters for a Multiphase Transient Flow simulation in a turbine.

Until now, everything seems to go fine except for one condition: I don’t know how to establish a CONSTANT water level in time downstream the rotor. As Initial conditions I configured the volume of fraction as:

WaterVF: if(y<Waterlevel,1,0)
Waterlevel:-200 mm
AirVF: 1-WaterVF

(Rotor=rotary domain, Rest=stationary domain)

But as time passes by, the water level decreases until I loose it completely. This is expected, since y have a downstream OUTLET (average static pressure -20kpa ) but how can I solve it?


I annexed 2 printscreens: t=0 and some seconds after


Thank you all in advance.

[ghorrocks]

Isn't this simply saying that your exit pressure is too low? -20kPa sounds like a vacuum to me so no wonder it sucks

Work out what the pressure should be at your exit.

[armlic]

Hello ghorrocks,

True. I realized that specific input data was improper so I changed the boundary to Mass Flow (equal to the inflow). Also, I think a proper counter pressure just enough to handle that water column might work fine.

Thank you for your advice.
AL

[ghorrocks]

A mass flow inlet and mass flow outlet will not work either. First of all it is numerically ill-defined as the pressure level is not set. And secondly, as a numerical solution is approximate then the inlet flow will not EXACTLY match the outlet flow then you will get a small flow imbalance and this will slowly either fill or empty the domain.

You need to apply a pressure at the outlet equal to the static head of the water column height you want. You are going to have to correct it for the reference density static head as well - have a look at the flow over a bump tutorial for an idea of how to do this.

[armlic]

Hello, ghorrocks

Now I configured an Outlet with Pressure equal to the water table, I still need to correct it, but so far is looking very good.
Thank you for the advice!