CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

CFX 5.4 Developing flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 27, 2000, 10:44
Default CFX 5.4 Developing flow
  #1
Bobby Malone
Guest
 
Posts: n/a
Has anyone looked at how CFX ( I am using version 5.4) handles developing flow? I have set up a simple long pipe under steady state conditions and calculated the blockage factor vs. L/D along the pipe. Compared to published data, "Klein 1981", I get rather bad results. I get a max. value of about 0.05 compared to typical results of about 0.15 to 0.2. I have so far only tried the ke model. Thanks.
  Reply With Quote

Old   September 27, 2000, 20:34
Default Re: CFX 5.4 Developing flow
  #2
John C. Chien
Guest
 
Posts: n/a
(1). How is your mesh distributed? (2). The pipe developing flow starts with zero boundary layer thickness at the entrance, which requuires the special mesh arrangement, that is, you need to squeez the mesh lines very close to the wall. And at the same time, the spacing near the entrance in the axial direction also need to be compressed in order to capture the rapid development of the boundary layer . (3). Lower blockage means less boundary layer effect. This could be due to inadequate capture of the B.L. (4). Improvement in mesh density and distribution should give you better results, I hope. (k-epsilon equaton with wall function is all right for this application)
  Reply With Quote

Old   September 28, 2000, 11:52
Default Re: CFX 5.4 Developing flow
  #3
Bobby Malone
Guest
 
Posts: n/a
In response to your question. The solid is a 30 degree pie segment from a 5 inch dia. pipe. A symmetric boundary is used on both sides. The length is 50 L/D. Unable to get thinner slice due to grid generation errors. Max edge length 0.16 inches. Angular resolution, 10 degrees, .02 min edge, .16 max edge, 1.3 expansion. Inflation on OD, 3 layers, 1.1 expansion, 1.5 thick multipler. Approx. 250000 nodes. Y+ about 35 on OD at Re=160000. ke converged 10E-5, 2nd order, 0.01 conservation, 0.001 time step.

If these parameters are not satisfactory, do you have a suggestion?

Thanks
  Reply With Quote

Old   September 28, 2000, 12:19
Default Re: CFX 5.4 Developing flow
  #4
John C. Chien
Guest
 
Posts: n/a
(1). The blockage is a function of the velocity profile only. So, your fully-developed profile must be very flat. (2). 250,000 is a good number. And if you have enough mesh points in the radial direction, say 30 points, then you also should get some reasonable numbers. (3). Run a couple of cases with different pie angles, for a shorter duct.(if 250,000 is the upper limit. you can cut the pipe shorter.) And check the results to see if it is related to the use of pie geometry and the related boundary conditions. A full 360 degree pipe would be ideal. (4). The angular resolution of 10 degrees and a total of 3 layers ( I hope I am reading it right) for a 30 degree pie shape is probably not adequate. Also check the type of symmetry condition used. Otherwise, plot the fully-developed profile against the published pipe profile to see the difference in the profile shape. You can also look at the profile of the tke and the eddy viscosity distributions.
  Reply With Quote

Old   October 3, 2000, 23:27
Default Re: CFX 5.4 Developing flow
  #5
joecfd
Guest
 
Posts: n/a
- Throw a couple more layers in the inflation.

- Sounds like you might be using an inlet/outlet setup. A better way is to shorten up your pipe, drive the flow with a momentum source and use a translational periodic boundary condition on the ends of the pipe instead. Then you should not have to use so much length.

- With a shorter pipe you should be able to use more resolution (radially) across the pipe now. So you answers should improve.
  Reply With Quote

Reply

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
How to Check Mass Flow Rate in 2D Analysis - CFX nasir FLUENT 0 October 9, 2011 02:52
How to set pulsatile flow in cfx? bmdaortiz CFX 4 September 8, 2009 22:48
compressible flow in CFX! Ihsan CFX 9 January 15, 2008 19:50
Define outlet with varying flow reistance in CFX Coriolius CFX 1 October 29, 2004 17:31
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 17:11.