Re:Fully developed flows!

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 June 30, 2003, 04:58 Re:Fully developed flows! #1 Miko Guest   Posts: n/a Hi all! If I wish my result is fully developed flows, how can I achieve this? Do I need build the domain, such as the duct, long enough, so I can hope that the region sufficiently far from the inlet is what I need? Thank you! Best regards! Miko

 June 30, 2003, 10:41 Re:Fully developed flows! #2 Louwrens Guest   Posts: n/a Yes, unless you know the fully-developed profile. if you do, you can specify this as a function on your inlet.

 June 30, 2003, 21:46 Re:Fully developed flows! #3 Miko Guest   Posts: n/a Hi Louwrens! Thank you again! According to physical analyse, we can know that the flow should be fully developed flows if the region is far from the orifice. I am wondering what did you mean. What kind of function can I specify on the inlet? You mean the velocity profile?

 July 1, 2003, 03:53 Re:Fully developed flows! #4 Louwrens Guest   Posts: n/a >What kind of function can I specify on the inlet? You mean the velocity profile? Yes, you can specify the velocity profile on the inlet using CEL, then you dont have to model a long entrance. You'll have to be sure that this is the "correct" velocity profile of course, and this you'd get from previous experimental data, for instance. otherwise you can specify one of the analytical profiles (ie quadratic for laminar flow, some form of power law for turbulent)

 July 1, 2003, 04:28 Re:Fully developed flows! #5 cfd guy Guest   Posts: n/a I think you can have two approaches: 1) The easiest one: Create a duct with a long length (L/D > 40 should be enough) and use a medium grid size, not too refined. And then you extract all required information on your post-processor. 2) Not so trivial: Create a small L/D duct, note that D is constant in your case, I think L/D < 1 should do, and set both "inlet-outlet" as periodic pairs. You can use a reasonable mesh size over the duct area and just 3 ou 4 nodes on the axial coordinate. Provide the required momentum source, paying attention on the correct mass flow(Re number), and you'll get your fully developed flow. The differences between those two? This first one is more computer and the second is more human time consuming. The results should be the same if you have the same grid size on the duct section. Regards, cfd guy

 July 2, 2003, 03:48 Re:Fully developed flows! #6 Miko Guest   Posts: n/a Hi Louwrens and cfd guy! Thank you! I think cfd guy's idea is suit for me. But I also have an idea: I will use User Fortran Subroutine to import the data of velocity profile at certain place from the first calculation as inlet velocity. I will continue doing so untill the velocity profile is stable. IS such doing right? Best regards! Miko

 July 4, 2003, 06:46 Re:Fully developed flows! #7 Bob Guest   Posts: n/a Hi CFD guy, using your second method, is the periodic inlet / outlet, when specifying the momentum source, do you need to use a function or something like that ? or do you specify constant momentum throughout the model ? Bob

 July 4, 2003, 07:26 Re:Fully developed flows! #8 cfd guy Guest   Posts: n/a Hi Bob, Unfortunately, I've been specifying a constant momentum source through the domain. I keep correcting it until I reach the correct massflow or Reynolds number. But you can use functions or generate scripts to do this for you. cfd guy

 July 4, 2003, 08:40 Re:Fully developed flows! #9 Bob Guest   Posts: n/a CFD Guy, I'm sure you could do something clever with perl to itereate to your required mass flow rate ? Do you then extract the velocities K and Epsilon to use as your inlet conditions ?

 July 4, 2003, 08:50 Re:Fully developed flows! #10 cfd guy Guest   Posts: n/a Yeah, you should do some scripting in complex flows. It's up to you. :P Answering the second question: Yes.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Maarten de Jong Main CFD Forum 7 April 30, 2012 02:23 SMM STAR-CD 3 September 9, 2011 15:54 SMM STAR-CD 0 September 5, 2011 22:08 SMM STAR-CD 3 August 29, 2011 11:38 Vidar Main CFD Forum 0 September 18, 2008 05:05

All times are GMT -4. The time now is 22:38.

 Contact Us - CFD Online - Top