[hiep.nguyentrong]

Hi, i have some problem with flow in pipe
My case is an ideal gas flow in pipe (0.4 m diameter and 2m length).
150m/s velocity inlet and pressure outlet with 0 gage pressure. i used k-esilon model.
The problem is pressure drop from 670 pa (inlet) to 0pa at outlet and velocity increase from 145 at inlet and 153 at outlet.
can anyone explain that.

[flotus1]

Several possible reasons, in no particular order:
1) Conservation of mass. As pressure drops towards the end of the pipe, velocity has to increase in order to transport the same amount of mass.
2) Transient phenomena with compressible effects. If there is a pressure wave within the pipe, you can have different mass flow rates at inlet and outlet. This does not violate conservation of mass. The mass difference is just added or subtracted to the mass in the pipe
3) Viscosity. As the flow travels through the pipe, a velocity profile develops with higher velocity in the center. Since you don't state how you post-processed velocities, it could max values.
4) Invalid solution. With 150m/s as a boundary condition you should get 150m/s at this boundary, not 145m/s.

Edit: or which part of the result was unexpected?

[hiep.nguyentrong]

Originally Posted by flotus1

Several possible reasons, in no particular order:
1) Conservation of mass. As pressure drops towards the end of the pipe, velocity has to increase in order to transport the same amount of mass.
2) Transient phenomena with compressible effects. If there is a pressure wave within the pipe, you can have different mass flow rates at inlet and outlet. This does not violate conservation of mass. The mass difference is just added or subtracted to the mass in the pipe
3) Viscosity. As the flow travels through the pipe, a velocity profile develops with higher velocity in the center. Since you don't state how you post-processed velocities, it could max values.
4) Invalid solution. With 150m/s as a boundary condition you should get 150m/s at this boundary, not 145m/s.

Edit: or which part of the result was unexpected?

1) the problem is pressure drop too high. This must be 535 pa when i used this equation dp = 7.57 q1.85 L 104 / (d5 p) . When im increase velocity to 0.8M, the diffirence inrease to 6 times (6kpa and 1kpa).
3) the boundary layer <5% and all the velocity at all point in outlet face is the same (1% diffirent).
4) this must have pressure at inlet, so the fluid can move from inlet to outlet. But fluent will ignored when flow is subsonic. So how i can fix the velocity at inlet. In my case, i think a part of dynamic pressure come to static pressure at inlet and convert all to dynamic pressure at outlet. i dont know what should i do.

ref of equation:https://www.engineeringtoolbox.com/p...pes-d_852.html

[flotus1]

this must have pressure at inlet, so the fluid can move from inlet to outlet.

I don't quite get that

Other than that, the formula you are referring to is most likely based on at least 2 assumptions: fully developed flow and fully developed turbulence. Maybe even more.
Your CFD model would have to account for this. Just two examples: Velocity at the inlet of your simulation will likely be a uniform profile, leading to much higher shear stress than in a fully developed flow. This in turn leads to higher pressure drop. And you would have to choose turbulence quantities at the inlet very carefully to match a fully developed turbulent flow.
And even then, the formula you are comparing to seems to be empirical. So some discrepancy is to be expected, even when being very careful with the CFD setup.

Based on your observation that the discrepancy increases with higher Mach numbers, one could conclude that the formula you are comparing to is based on a third assumption: low Mach number or small pressure differences.
The note a little further down confirms this suspicion:

NOTE! - a pressure drop above 1 kg/cm2 (14-15 psi) is in general not relevant and the formula and calculators above may not be valid.

For a more accurate calculation - or for a longer pipe lines with larger pressure drops - divide the line in parts and calculate the pressure drop and final pressure for each part. Use final pressures as initial pressures for the next parts. The final pressure after the last part is the final pressure at the end of the pipe line. The pressure drop for the whole pipe line can also be calculated by summarizing the pressure drops for each part.

[hiep.nguyentrong]

Originally Posted by flotus1

I don't quite get that

Other than that, the formula you are referring to is most likely based on at least 2 assumptions: fully developed flow and fully developed turbulence. Maybe even more.
Your CFD model would have to account for this. Just two examples: Velocity at the inlet of your simulation will likely be a uniform profile, leading to much higher shear stress than in a fully developed flow. This in turn leads to higher pressure drop. And you would have to choose turbulence quantities at the inlet very carefully to match a fully developed turbulent flow.
And even then, the formula you are comparing to seems to be empirical. So some discrepancy is to be expected, even when being very careful with the CFD setup.

Based on your observation that the discrepancy increases with higher Mach numbers, one could conclude that the formula you are comparing to is based on a third assumption: low Mach number or small pressure differences.
The note a little further down confirms this suspicion:

Thank you so much. Your answer is helpful for me