CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

pressure losses in pipes

Register Blogs Members List Search Today's Posts Mark Forums Read

LinkBack Thread Tools Display Modes
Old   February 1, 2007, 07:32
Default pressure losses in pipes
Posts: n/a
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

  Reply With Quote

Old   February 2, 2007, 06:54
Default Re: pressure losses in pipes
Posts: n/a
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.

  Reply With Quote

Old   February 2, 2007, 10:42
Default Re: pressure losses in pipes
Posts: n/a
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
  Reply With Quote

Old   February 5, 2007, 13:33
Default Re: pressure losses in pipes
Andy R
Posts: n/a
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
  Reply With Quote


Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Maintaining Static Pressure at Fluid Flow Inlet cdevalve FLUENT 3 January 14, 2012 01:11
pressure inlet & outlet. help ASAP Plz engahmed Main CFD Forum 0 June 13, 2010 15:34
Help ASAP! pressure inlet & outlet engahmed FLUENT 0 June 13, 2010 15:33
resistance & pressure losses Jan CFX 0 May 14, 2002 07:33

All times are GMT -4. The time now is 01:12.