CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Phoenics (http://www.cfd-online.com/Forums/phoenics/)
-   -   fully developed turbulent flow in a pipe (http://www.cfd-online.com/Forums/phoenics/51088-fully-developed-turbulent-flow-pipe.html)

Dipak July 18, 2000 00:36

fully developed turbulent flow in a pipe
 
Dear all, I refer library case no. 502 where fully-developed turbulent flow and heat transfer in a circular pipe at a Reynolds number of 1.E5 and a Prandtl number of 3.0 has been considered. Running this case i'm not getting the reported f(0.018) and Nu(393) values. Would anyone kindly look into the matter as it is related to the implementation and applicability of k-e model in phoenics??

Thanks in advance. Dipak

Mike Malin July 18, 2000 10:43

Re: fully developed turbulent flow in a pipe
 
I am not sure what release you are using, but PHOENICS V3.3 produces the correct RESULT.

Presuming that you have put ROUGH=F so that you are simulating an hydraulically smooth wall, then you should find from the RESULT file that the near-wall axial velocity W1 is 0.6549 and that the dimensionless LOCAL wall shear stress SKIN (=(W*/W1)**2) is 4.968E-3. Then f can be computed as:

f = SKIN * 8 * (W1/Wb)**2

where the bulk axial velocity Wb = 1.0. Thus, f=0.0171, which is pretty close to 0.018.

The friction factor can be computed in a number of other ways from the RESULT file, including from the pressure drop dp/dz which is printed as 8.520923e-02 in the RESULT file, i.e. via

f = dp/dz/(0.5*rho1*Wb**2)/D

I won't do the algebra for the Nusselt number, but one way is to compute from Nu=St*Re*Pr based on bulk properties. The LOCAL Stanton number is printed as STAN in the RESULT file, and so as with SKIN above, you will have to convert STAN from a LOCAL quantity based on near-wall properties to a value based on bulk properties.

Dipak July 20, 2000 01:42

Re: fully developed turbulent flow in a pipe
 
Hi Mike, Thanks for your reply. I'm using PHOENICS 3.2 that gives similar results as you have found from PHOENICS 3.3. I also did the calculation in a similar way. Though i find f value 0.01704 like you, but the Nusselt number comes very diffrent. Here the algebra for NU:

St = STAN*W1(NY)*(TW-TEM1(NY))/[WB*(TW-TB)] Nu = Re*Pr*St where, W1(NY)=0.6549, TEM1(NY)=6.408

WB=1.0, TB=5.285946, TW=10.0

STAN = 2.529E-3, Pr=3.0, Re=1.0E+5 So, Nu comes 378.6 which should be 392.

Waiting for your reply. Thanks in advance.

Dipak

Mike Malin July 20, 2000 05:53

Re: fully developed turbulent flow in a pipe
 
I agree with your result, but I would suggest that the difference is not significant from a practical point of view because of the scatter in the experimental data. For example, other correlations yield different values of Nu.

The Q1 file was created on a much earlier version of PHOENICS, and I suspect that internal changes in EARTH are responsible for the different predictions. For example, the use of default harmonic or arithmetic averaging in the turbulent diffusion terms of the field variables may have an influence, as can the values used for the log-law constants. These have changed during the life of PHOENICS, but seems the comments at the top of the q1 file have not.

The log-law constants used are k=0.41 and E=8.6. The prediction of f=0.017 rather than 0.018 is not really disturbing, as again this is within the scatter of the data. You can check the near-wall value of velocity obeys the log law if you doubt the predictions. It follows that the near-wall turbulence values can also be checked because they scale with the friction velocity.

I would suggest that the turbulent Prandtl number PRT(TEM1) ought to be around 0.9 rather than the 1.0 default used in the Q1. This will lead to a larger value of Nu.

If you doubt the model thermal predictions then check that the predicted near-wall temperature obeys the logarithmic temperature law for which the P-function employed by PHOENICS is the one proposed by Launder & Spalding as a simplification of the more complex Jayatilleke P-function.

I recall participating in a turbulence workshop organised by Peter Bradshaw of Stanford University and a later and more recent one by Andrew Pollard of Queens University, Canada. it may be of inetrest to you that an interesting outcome of these workshops was the widely differing results produced for f and Nu for the pipe flow by the various participants, which included several CFD vendors. This case was only meant to serve as a precursor to more complex cases.

I hope this helps.


All times are GMT -4. The time now is 04:57.