Hi

I am trying to simulate (in CFX 5) a case of wind flow around a large tank and some gas is leaking from the tank.

My problem is that I keep getting in flow at the out flow boundary (downstream)

I have a large box where the tank is placed inside. A wind velocity profile at the inlet. Symmetry on the side and top. At the downstream outlet boundary I have tried opening (Relative pressure of 0.0) and outlet (Static pressure = 0.0).

I presume that the problems lies in the outflow boundary, but what is going wrong ?

Any suggestions ???

Thanks. /Peter

Hi Peter,

You probably have a recirculation behind your tank, and your exit boundary cuts through the middle of it. This means there will be sections of reverse flow at the plane you chose. You can either:

1) If accuracy of the recirculation is not important you can make your exit an opening and the boundary will handle (in a crude way only) the reverse flow.

2) If accuracy of the recirculation is important your only option is to move the exit boundary further downstream. If you are using a high Reynolds number (and a tank in atmosphere would be high Reynolds number) then this recirculation can persist a long way downstream. How far downstream do you currently have the exit (relative to the size of the tank)? I would suggest placing the exit boundary at least 20 times the size of the tank downstream.

Another possibility is it is the flow doing strange things before it reaches convergence. In this case you can improve the situation by specifying a better initial guess (eg for this case setting an initial velocity across the entire domain should do).

Regards, Glenn

Hi

The size of the tank is 140 m in diamnter and 28 m in height.

The domain after the tank is 590 m. The outflow boundary is an opening (relative pressure = 0.0).

The rms residual of uvw momentum and p-mass is less than 1.0e-04. The case is run as non-isothermal due to bounancy of the gas.

/Peter

Glenn, If buoyancy were being used and the domain is very large, do you think that the pressure on the down stream boundary would have to be a function of the hydrostatic pressure ?? Another possible way around this would be to specify an opening ont he down stream boundary condition, and define the velocity profile (same as your inlet). However hear you would be assuming that the domain is sufficiently large that the Atmospheric boundary layer profile has reccovered and is not affected by the wake of the tank. This way the pressures on the boundary should sort themselves out (or at least thats how I understand it ?). Bob

Hi

I am not sure about the hydrostatic pressure at the outflow boundary.

I was is woundering me is that at the outflow I can see a gradient of the pressure even though I have set the opening boundary with a relative pressure of 0.0.

At the top of the outflow boundary the pressure is 0.0 Pa (Relative), closer to the ground the relative at the outflow start to increase and have a max close to the ground with -872 Pa. (flow into the domain).

I am running out of suggestion.

/Peter

Hi Peter,

If you including the effects of buoyancy/gravity you will need to vary the pressure with height in your exit boundary (as Bob said).

You said the tank has a diameter of 140m and your exit boundary is 590m downstream. This means you are only going downstream about 4 diameters. This is definitely too close if you want to accurately resolve the recirclation. Move it at least 10 diameters downstream for a rough solution, or 20 or more if you want good accuracy.

Regards, Glenn