Learning Forum

[martinwagar]

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, k-epsilon model using standard wall functions.  The problem still exists if I use mass-flow-inlet instead of a velocity-inlet.  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 1e-6.

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

 

[singh33]

Dear Ryan,

I too have solved this problem with both K-e model and K-w model, the thing you should take into mind is when using k-w model you go for the inflation layer concept and for standard wall function approach or the k-e 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 k-e model not for K-w) which can reduce your overall mesh count,

secondly, realizable K-e is for swirling flows where Swirl no, < 0.5  for your simple pipe flow case you should use standard K-e 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.

[martinwagar]

Thank you for your quick response!  

In switching to the k-w model (standard), the issue has been resolved and has very good agreement with the analytical solution (28 kPa) 

# of divisions   k-e pressure drop   k-w 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 k-e model work.  I'll update here if successful.

Again, I appreciate your quick response!

Ryan

[Karthik Remella]

 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