Hi,

i think i have a stupid question for you all: i need to simulate a pipe with outflow in atmosphere. i know the total pressure at inlet.

Is it correct to impose a static pressure of 1 atm at the output section of the tube or should i have to model a big external plenum where to impose the pressure of 1 atm?

i make this question because in my opinion it is not physically correct to impose the atmospheric pressure at the output section of the tube, because the flux expand outside the tube and reach the pressure of 1 atm faraway the output section of the tube.

Am i correct? What is the correct boundary condition?

Thank you very much and excuse for my bad english.

It is better to put a mass flow BC at bube outlet. Well, that is not you wanted and you did not know the mass flow. So, if you are only interested in the flow inside the tube, then it is ok to put 1 atm static pressure at tube outlet. If you need to simulate the jet flow, that is totally a different story.

Hi Miry,

Firstly, remember that your outlet pressure is defined relative to the domain reference pressure. If the reference pressure is 1 [atm], your outlet pressure should be zero.

If there is a sudden expansion at the end of the pipe, the static pressure at the plane of the pipe will be nearly constant, so applying a constant static pressure would be a reasonable assumption. Do no use the "Average Static Pressure" option in this case.

I wouldn't recommend a mass flow boundary condition in this case, since you would not get the right back pressure. If your inlet total conditions are accurate, the static pressure option is the right way to go.

That said, if you have a sudden expansion and you wish to use a mass flow rate at your outlet you should use the Mass Flow Update option "Shift Pressure" and specify a constant value for the pressure profile (any value will do). The solver will apply the pressure profile you provide and shift it up or down to acheive the specified mass flow rate. The advantage here is that you end up with the right pressure profile.

-CycLone

Thank you all.

What i wanna tell is that if you impose a static pressure of 0 Pascal at outlet (1 atm as reference pressure) and a mass flow at inlet, the software calculate for the inlet a pressure that is not realistic.

In fact at the outlet section, the real static pressure of the fluid is not zero but a value greater than zero.

Hi CycLone

i have one big doubt i am doing one inlet plenum analysis. My BCs are Total pressure at Inlet(i set reference pressure is Total pressure, inlet Bcs is zero pressure) Mass flow rate at outlet.

After solution converges i have seen a pressure plot.

But CFX shows Total pressure inside the plenum is higher than what i specified in the inlet of the plenum.

How is it possible. because we didnt add any energy inside. some cases static pressure itself shows higher than Total pressure specified in the inlet.

Please tell me how i beleive the answer

Thanks in Advance kathiravan

Hi Kathiravan,

This often indicates numerical error and the problem should go away, or at least minimize with mesh refinement.

In a viscous flow it is physically possible to locally have a total pressure greater than your inlet total pressure. This actually occurs at a stagnation point where the fluid on either side is imparting a shear stress on the stagnating streamline in the same direction, thus locally imparting energy to the fluid, while globally the average total pressure still at or lower than the inlet level.

The region of locally higher total pressure can be quite large at very low Reynolds numbers, but rapidly shrinks as the Reynolds number increases. However, due to the formulation of turbulence models in CFD, which essentially add a turbulent viscosity to the dynamic viscosity, it is possible to see the same effect at large Reynolds numbers because the effective Reynolds number (based on the effective viscosity) is actually quite low.

Furthermore, the effect can occur with two equation turbulence models in regions of accelerating flow. Accelerating flow results in an increase in shear strain rate which in turn results in the production of turbulence. This is a by-product of the assumptions of the model and there are limiters to minimize the effect. The SST model has such a limiter on by default, so switching to SST may help. I think there is also the Kato-Launder limiter function in k-epsilon that you can also try, but it is more problematic than the SST implementation.

Hope this helps.

-CycLone

[Er.spcwlkr]

How to consider what option we have to select and what change it will make please God help me am dealing with horror dreams while working with ansys fluent

[ghorrocks]

This is the CFX forum. If you are having horrible dreams about Fluent then try the fluent forum.