Verification of Power-law fluid annular flow problem

[Anonymous]

Hi

I am trying to model annular flow of a power-law fluid using Autodesk Simulation CFD. The results that I get from the software are different from hand-calculated ones. For hand calculation, I am using Hanks and Larsen’s proposed equation which relates flow rate to the pressure drop along an annulus. Below are the parameters I am using for my simulation:

Power law model: n=0.5, k=0.5 pa.sec^n  

Annulus OD= 0.3 m,  annulus ID= 0.2 m

Q= 20 kg/sec  fluid density=1200 kg/m^3

Hand calculated pressure drop: 164.4074 pa/m

CFD model prediction: 348 pa/m

The link for CFD simulation files access: https://www.dropbox.com/sh/hhwzfdhorjy3r5h/AACxyWg8YbOfRDSqpiaSsA1ha?dl=0

 Link for Hanks and Larsens equation explanation:  https://www.dropbox.com/s/gzqql0txfciieuz/Hanks%20and%20Larsens%20flow%20rate%20equation.pdf?dl=0

Thanks a lot in advance for your help

[srhusain]

The (.cfdst) file is not useful in opeining your moedl. You need to post or attach the support file <studyname>_support.cfz- rename it to <studyname>_support.zip and then attach this or place in box.

[Anonymous]

Thanks for your response 

I am attached the file. I noticed that the problem might be with meshing pattern since for my case it highly affects the pressure drop prediction.

[srhusain]

I have attached a modified version of the suppport file with the changes:

1. Use extruded mesh for better accuracy
2. Change advection acheme to Adv5

The overall pressure drop is around 931 Pa for the total length of 5 meters, which amounts to roughly 186 Pa/meter, an "error" of +13.3% over the hand calculation. Note that the cross section mesh is still very coarse and you may want to refine that.

Anoth point of note is that the error is likely a bit less because a portion of the pipe is developing flow, which incurs a higher pressure drop

An alternative is to try an axisymmetric model

Hope this helps.

[Anonymous]

Thanks a lot srhusain

Your comments were really helpful. Regarding your comment about the portion of the annulus with developing flow, I tried to eliminate the effects of developing flow by assigning volume flow rate, instead of mass flow rate, to the annulus inlet and then checking the box “fully developed“. But, the software says the option of fully developed flow can’t be applied to the annulus surface. Do you have any idea how to deal with this problem in order to eliminate annulus inlet effects?

Regards

[srhusain]

A simple way to deal with this is to make the pipe length large enough to account for the entry length and use the fully developed region for measurement of pressure-drop.

Another way is to impose the known pressure drop as an inlet boundary condition. For example, the total pressure drop is around 164 x 5 = 820Pa for the 5 meter pipe, so apply 820 Pa at the inlet, 0 Pa at the exit, and see if you get the expected flow rate.

[Anonymous]

This time I am trying to model annular Couette flow of a Power-law fluid, where the inner cylindrical bounding surfaces is moving longitudinally at a constant rate of V=0.2 m/s. The model parameters are the same as defined above for the non-Couette flow case. For this case, I increased the model length to 40 m and used extrusion for meshing the model as “srhusain” recommended before to do so. The analytical solution for this problem gives dp= 88.98 pa/m while the software prediction is 163.74 pa/m. For analytical solution equations (8) and (9) in the attached paper has been implemented. Also, the velocity disribution at the annulus inlet has a weird shape.

Thanks