[Naveenjanj]

I am trying to solve Ansys Verification Manual number 28 using
Fluent 2D Axisymmetric option.

The title is “Flow and Heat Transfer Over Expansion Pipe”

In this manual I am having doubt as how to choose Hydraulic diameter for inlet and outlet boundary condition.

What should be the inlet boundary condition?
Outlet boundary condition??

Could anyone tell me the correct b/c ?

[vinerm]

Since the problem is axisymmetric, actual diameter at the inlet is the hydraulic diameter; same is true for the outlet.

As far as outlet is concerned, pressure outlet is alright. However, for the inlet, you have to develop a profile and use that. You need to run a case with only inlet duct (no expanded portion) and then extract a fully-developed velocity profile from there. Then apply that profile in this simulation.

[Naveenjanj]

Originally Posted by vinerm

Since the problem is axisymmetric, actual diameter at the inlet is the hydraulic diameter; same is true for the outlet.



As far as outlet is concerned, pressure outlet is alright. However, for the inlet, you have to develop a profile and use that. You need to run a case with only inlet duct (no expanded portion) and then extract a fully-developed velocity profile from there. Then apply that profile in this simulation.

Hi,

May I know how to extract a fully-developed velocity profile. Could you please elaborate.

[vinerm]

There are two options. One is to create a pipe with diameter of your first pipe. Ensure that it is long enough so that the profile gets developed. Run the case with the specified velocity inlet and pressure outlet. After the simulation has converged, write profile using File > Write > Profile > Define New Profile at the outlet for all three velocity components.

Another option is to create a pipe with the diameter of the first pipe, however, the length can be just a few mm or cm. Ensure that there are at least 5-6 cells across length. Then setup inlet and outlet as translational periodic boundaries. Apply periodic settings and assign either flow rate or pressure drop. Run the simulation. Once done, extract profile at either of the boundaries. This option is more sophisticated but you need to know Fluent little more than you may know at this stage. So, you may use first option.