CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   pressure losses in pipes (http://www.cfd-online.com/Forums/fluent/43581-pressure-losses-pipes.html)

lottie February 1, 2007 07:32

pressure losses in pipes
 
Hi I am trying to calculate the k factor from my fluent model from the pressure losses in pipes and the density and velocity of the fluid in a pipe. The k factors I have calculated are larger than those calculated theoritically. Does anyone have any ideas what I am doing wrong or ideas to try. Thanks


gurion February 2, 2007 06:54

Re: pressure losses in pipes
 
You should check that your Fluent model reconstructs your theoretical calculation:

laminar or turbulent flow

isothermal or adiabatic walls

entrance and exit boundary conditions

It would help if you stated this data in your post.


lottie February 2, 2007 10:42

Re: pressure losses in pipes
 
I am working with laminar flow and aim to use turbulent once the laminar is sorted. I am not using either isothermal or adiabatic walls. I have an entrane boundary condition of velocity of which I change. I have not set any exit boundary conditions. What would be going wrong? thanks lottie

Andy R February 5, 2007 13:33

Re: pressure losses in pipes
 
K factors as reported in engineering literature are based on tests which include long upstream sections. Thus regardless of whether the flow is laminar or turbulent, it will be FULLY DEVELOPED. If you apply a fixed constant velocity profile (as I suspect you have) you will not be duplicating the conditions upon which K was determined. My own analyses of pipe components with fully turbulent flow is that the fixed velocity condition results in about a 10% overprediction of the delta p and thus K. I am not sure if that would not be an even larger effect for simple pipe flow

You can

A. Figure out from pipe flow equations the distance required for fully developed flow and add that to your model

B. Use the repeating boundary condition on a small pipe model using your grid spacing. When this converges you can export this as a profile and apply it to your detailed model. If you are doing straight pipe you can use this BC directly on your grid.

Ultimately I would not expect to get much closer than +/- five percent to a K-factor from something like Crane. Small details in a fitting which result in gaps and steps can have an observable effect on the DP at least of the CFD solution. You would need the detailed drawings of the component in question to model to. Additionally how was the measurement taken? A single wall static tap may give a different value than if a series of taps around the circumference are averaged, or piped to a common manifold.

Also remember that those K factors are the result of many tests possibly on different geometries which have been manipulated to be a single value.

I would only look for very close matches for

A. Problems that have a well defined closed form solution with only limited empirical constants

B. A test where you know all the details of the geometry and how it was performed.

Good Luck - Andy R


All times are GMT -4. The time now is 19:03.