[FrostRay]

Hello guys!

I am currently trying to do a simulation for a micro-scale laminar pipe flow on Ansys Fluent. One main step of which is to try a simulate a 3D pipe flow, then compare the simulation results to theoretical results (Poiseuille's Law).

Now, the problem is the pressure drop values I obtained from Ansys are significantly higher (about 30-40% higher) than the theoretical values.

For example, a mass flow rate at the inlet of 12 µL/s will have a theoretical pressure drop of 76 kPa. But my simulation results show 110 kPa, which is 40% higher.

Information on 3D pipe:
• Diameter: 4 x 10^-5 m = 0.040 mm = 40.0 µm
• Length: 4 x 10^-4 m = 0.40 mm = 400.0 µm
• Thickness: 5 x 10^-6 m = 0.005 mm = 5 µm

Setup Settings:
• I created and meshed a 3D cylinder - with inlet, outlet and wall as boundaries
• Laminar flow
• No-slip wall
• Fluid used is water

• Inlet boundary condition: Mass Flow Rate (eg: 12 µL/s, 16 µL/s)
• Outlet boundary condition: Pressure outlet (0 Gauge Pressure)

• Mesh is very fine (500,000 cells)

• Solution method: SIMPLE
• Initialization: Hybrid

Calculations for Fluid Flow:
• Reynold's Number = 382.02
• Average Velocity = 9.55 m/s

Any insights and suggestions? What could have possibly gone wrong with my settings?

Thank you so much for your help.

[evcelica]

Could be many things, first guess:
The velocity profile at the beginning (near the inlet) is not fully developed, FLUENT probably brings it in at a uniform velocity, so dP/dx would be larger than if fully developed.
do a longer pipe and calculate dP/dx away from the inlet after the velocity profile is fully developed.

[CFDKareem]

Originally Posted by evcelica

Could be many things, first guess:
The velocity profile at the beginning (near the inlet) is not fully developed, FLUENT probably brings it in at a uniform velocity, so dP/dx would be larger than if fully developed.
do a longer pipe and calculate dP/dx away from the inlet after the velocity profile is fully developed.

I second this. The entrance length can be calculated as L = 0.05*Re*D, for laminar flow. In your case the fluid velocity is around 9.5 m/s, Reynolds number is approximately Re=380, and the hydraulic diameter is D=40 um. Therefore the expected entrance length would be ~760 um. You can double check my math, but it is likely that your entire pipe is inside the entrance length. Therefore, the pressure drop is going to be much higher than expected.

You can try using a fully developed flow profile at the inlet to "skip" the entrance length. This should match your calculated value much closer. Or you can find the pressure drop correlation which takes into account the pressure drop defect of the entrance length.

[FrostRay]

Originally Posted by evcelica

Could be many things, first guess:
The velocity profile at the beginning (near the inlet) is not fully developed, FLUENT probably brings it in at a uniform velocity, so dP/dx would be larger than if fully developed.
do a longer pipe and calculate dP/dx away from the inlet after the velocity profile is fully developed.

Hi thank you for your response! I will increase the length of the pipe and run the simulations again.

[FrostRay]

Originally Posted by CFDKareem

I second this. The entrance length can be calculated as L = 0.05*Re*D, for laminar flow. In your case the fluid velocity is around 9.5 m/s, Reynolds number is approximately Re=380, and the hydraulic diameter is D=40 um. Therefore the expected entrance length would be ~760 um. You can double check my math, but it is likely that your entire pipe is inside the entrance length. Therefore, the pressure drop is going to be much higher than expected.

You can try using a fully developed flow profile at the inlet to "skip" the entrance length. This should match your calculated value much closer. Or you can find the pressure drop correlation which takes into account the pressure drop defect of the entrance length.

Hey thank you for your response!

If so, the entrance length will be L = 0.05(Re)(D) = 0.05(382.02)(0.00004 m) = 7.64 x 10^-4 m > Pipe length of 4 x 10^-4 m

Yes, your calculations are correct.

For the methods you suggested,

1) How do I create a fully developed flow profile at the inlet to "skip" the entrance length?

• Do I use a equation and increase the mass flow rate at the inlet?
---> But increasing mass flow rate at the inlet will cause pressure drop to be even higher

2) How do I find the pressure drop correlation which takes into account the pressure drop defect of the entrance length?

• Do I use Poiseuille's Law to calculate the pressure drop using the entrance length of 7.64 x 10^-4 m?
---> This will make the calculated pressure drop higher

Thank you so much for your help!

[CFDKareem]

Originally Posted by FrostRay

Hey thank you for your response!

If so, the entrance length will be L = 0.05(Re)(D) = 0.05(382.02)(0.00004 m) = 7.64 x 10^-4 m > Pipe length of 4 x 10^-4 m

Yes, your calculations are correct.

For the methods you suggested,

1) How do I create a fully developed flow profile at the inlet to "skip" the entrance length?

• Do I use a equation and increase the mass flow rate at the inlet?
---> But increasing mass flow rate at the inlet will cause pressure drop to be even higher

2) How do I find the pressure drop correlation which takes into account the pressure drop defect of the entrance length?

• Do I use Poiseuille's Law to calculate the pressure drop using the entrance length of 7.64 x 10^-4 m?
---> This will make the calculated pressure drop higher

Thank you so much for your help!

1) You'll use the equation for a parabolic fully developed profile where V_average = V_max/2. V_max will be the velocity at the inlet for the given mass flow (~9.5 m/s for your case). You can now create the parabolic profile using either a UDF or expression. Here is a video on how to apply this with expressions https://www.youtube.com/watch?v=oXbfD7GdX9k

2) The analytical equation of pressure drop including the entrance effects gets a little complicated (friction factors, etc.). Chapter 3 of this book https://www.sciencedirect.com/book/9...-microchannels has a great explanation of the calculation. If you can't find a PDF version, you can definitely find the same equations online somewhere.

[CFDKareem]

For reference, the equation your looking for will take the form:

[FrostRay]

Originally Posted by CFDKareem

For reference, the equation your looking for will take the form:

Hi can this equation be used for a aluminium pipe wall, no-slip wall, with dimensions from my starting post?

This equation contains friction factor, f.

Or do I need to add in friction condition in the simulation setup on Ansys Fluent? If so, how should I proceed on doing it?

Thank you!

[CFDKareem]

Originally Posted by FrostRay

Hi can this equation be used for a aluminium pipe wall, no-slip wall, with dimensions from my starting post?

This equation contains friction factor, f.

Or do I need to add in friction condition in the simulation setup on Ansys Fluent? If so, how should I proceed on doing it?

Thank you!

The friction factor comes from the viscosity and shear stress created by the no slip condition at the wall, so even with a smooth pipe you will have a friction factor. For a smooth, round, laminar pipe flow this can simply be written as:



where for fully developed flow in a circular pipe. The friction factor will change with roughness on the walls. For microchannels, even a small roughness value will contribute significantly to the pressure drop. So if you are trying to correlate to experimental data you may want to account for the roughness.