

March 31, 2020 at 3:58 pmmartinwagarSubscriber
Hi,
For a 2D axisymmetric pipe problem solved with double precision, I am getting a relationship between # of divisions in the radial direction of my mesh and pressure drop in the axial direction. The pipe is roughly 12 mm in diameter and 4.25 m long. My fluid is water moving at 2.3 m/sec at the inlet. I am solving with a realizable, kepsilon model using standard wall functions. The problem still exists if I use massflowinlet instead of a velocityinlet. All solutions used a coupled scheme with least squares for gradient and second order for pressure, momentum, TKE, and dissipation. All residuals are set to 1e6.
With 500 evenly spaced divisions in the axial direction (when varying spacing in the axial direction, there is virtually no relationship with pressure drop), here are the pressure drops I am seeing vs. the # of divisions in the radial direction.
# of divisions Pressure Drop (Pa)
10 24024
20 23594
30 22099
50 28701
100 36663
200 41802
300 43540
Ignoring entrance and exit effects, my analytical solution suggests a pressure drop of around 28 kPa.
Any help interpreting this dependency would be greatly appreciated.
Best,
Ryan

March 31, 2020 at 6:44 pmsingh33Subscriber
Dear Ryan,
I too have solved this problem with both Ke model and Kw model, the thing you should take into mind is when using kw model you go for the inflation layer concept and for standard wall function approach or the ke model you go for first cell height, I would suggest you to please calculate your 1 st cell height thoroughly and then use it for your problem, with first cell height successfully set you don want a cell growth (preferably for ke model not for Kw) which can reduce your overall mesh count,
secondly, realizable Ke is for swirling flows where Swirl no, < 0.5 for your simple pipe flow case you should use standard Ke only,
thirdly, how your calculating the mass flow rate, it should be calculated for the bulk mean temperature and then must be implemented,
fourth, when making mesh you should see that the biasing you use for the inlet will be reserved by default for the outlet and what you got is the transition of the inflation layer from pipe wall to the pipe axis, so you should reserve the direction of the biasing manually such that mesh density lie on the wall side or the first cell height lie on the wall side.
last is your axis symmetry condition are you taking the axis of the pipe as symmetry keeping the height of the 2 D surface as a radius of the pipe or the diameter, if you are using the diameter then you are wrong, you can visit CORNELL University lecture on CFD they have silver this problem excellently
Thanks & Regards.

March 31, 2020 at 8:09 pmmartinwagarSubscriber
Thank you for your quick response!
In switching to the kw model (standard), the issue has been resolved and has very good agreement with the analytical solution (28 kPa)
# of divisions ke pressure drop kw pressure drop
10 24024 26496
20 23594 26647
30 22099 27209
50 28701 28580
100 36663 29317
200 41802 28170
300 43540 28196
A few other notes:
For calculating the mass flow rate, I multiplied by volume flow rate by 999.4 kg/m3, the density of water at my operating temp. When looking at inlet velocity, I divided the volume flow rate by the cross sectional area of the pipe.
For the mesh, I had absolutely no bias in the radial direction and no bias in the axial direction. All cells were exactly 1/500th of the axial length and 1/nth of the radial dimension (where n is the number of divisions).
For the axis symmetry, I did use the radius of the pipe. All of my initial learning in Ansys was via the EDX course offered by Cornell, which didn't have any modules with turbulent pipe flow (only laminar). Are you referring to the module offered here (https://confluence.cornell.edu/display/SIMULATION/FLUENT++Turbulent+Pipe+Flow)?
Lastly, I do plan on using your comments to make the ke model work. I'll update here if successful.
Again, I appreciate your quick response!
Ryan

March 31, 2020 at 9:59 pmKarthik RAdministrator
Hello,
If you found the answer useful, please mark it as 'Is Solution'. I'm glad you were able to figure this out.
Good luck!
Best,
Karthik

 You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from lifesaving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Suppress Fluent to open with GUI while performing in journal file
 Heat transfer coefficient
 What are the differences between CFX and Fluent?
 Floating point exception in Fluent
 The solver failed with a nonzero exit code of : 2
 Difference between Kepsilon and Komega Turbulence Model
 Getting graph and tabular data from result in workbench mechanical
 Time Step Size and Courant Number
 Mesh Interfaces in ANSYS FLUENT
 error in cfd post

1862

1661

905

650

347
© 2022 Copyright ANSYS, Inc. All rights reserved.