[vronti]

Hello

I am simulating water flow through a rectangular duct (6x9x500)mm to get the fully developed flow; to use the output for a different simulation.
I ran the simulation for Reynolds Number - 500, 2000, 5000, 9000 using Ansys Fluent (realizable KE - standard wall functions) and OpenFOAM-v2006 (simpleFoam, realizable KE). I use OpenFOAM for complete task and ran fluent simulation to validate the OF results. I got similar results on both solvers.
But I thought Re-500 and 2000 is laminar flow and ran both solvers with laminar and found a rise in peak velocity of full-developed flow.

1. It is unclear for me since the simulation is plain flow through a duct.
2. In OpenFOAM, if I increase the length of the duct the maximum velocity is decreasing and I see more flatter profile for turbulent flow. But this doesn't seem to be the same for Fluent case. Why is it?
Any theoretical insight regarding this is greatly appreciated.

I attached the plots and openfoam case file (flowDevelop_500_2.zip) to recreate
Regards,
Screenshot 2022-07-11 221233.png
P.S:
Geometry: Rectangle : width - 6mm, height - 9mm, length - 100/500mm
Boundary conditions: Top Bottom - Walls, Sides - symmetry, velocity inlet, pressure outlet.
Solver - SIMPLE/ simpleFoam

[FMDenaro]

Originally Posted by vronti

Hello

I am simulating water flow through a rectangular duct (6x9x500)mm to get the fully developed flow; to use the output for a different simulation.
I ran the simulation for Reynolds Number - 500, 2000, 5000, 9000 using Ansys Fluent (realizable KE - standard wall functions) and OpenFOAM-v2006 (simpleFoam, realizable KE). I use OpenFOAM for complete task and ran fluent simulation to validate the OF results. I got similar results on both solvers.
But I thought Re-500 and 2000 is laminar flow and ran both solvers with laminar and found a rise in peak velocity of full-developed flow.

1. It is unclear for me since the simulation is plain flow through a duct.
2. In OpenFOAM, if I increase the length of the duct the maximum velocity is decreasing and I see more flatter profile for turbulent flow. But this doesn't seem to be the same for Fluent case. Why is it?
Any theoretical insight regarding this is greatly appreciated.

I attached the plots and openfoam case file (Attachment 90690) to recreate
Regards,
Attachment 90689
P.S:
Geometry: Rectangle : width - 6mm, height - 9mm, length - 100/500mm
Boundary conditions: Top Bottom - Walls, Sides - symmetry, velocity inlet, pressure outlet.
Solver - SIMPLE/ simpleFoam

First, if you assume a laminar 3D flow, a steady exact solution is simply obtained by solving the 2D Poisson equation for the stream-wise velocity on the rectangle. The source term depends on the Re number.


When you compare the laminar solution to the turbulent profile you have to consider you are evaluating the statistically averaged profile. Thus, the comparison must be made "congruent".

[LuckyTran]

1. What is the confusion? Laminar flows should yield the parabolic profile at any Re. Turbulent ones will produce the flatter profile.
2. Are you comparing the profile at the same station and seeing a change in the profile or are you comparing the profiles at the duct exit? Do both comparisons.


Personally I would recommend using cyclic and periodic boundary conditions to get the fully developed profile.



Please avoid the use of type fixedValue and value $InternalField as an inlet boundary condition for k or any other variable for that matter. This sets the inlet boundary condition for k to be the initial condition. If that sounds crazy it's because it is crazy.


I see you are using a uniform mesh. I recommend using some wall clustering strategies. Make your plots as points rather than lines, or superimpose the points so you can see where the actual data are. It should be apparent why uniform mesh is not-so-good.