# Fully developed flow boundary condition

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

 LinkBack Thread Tools Display Modes
 December 28, 2009, 10:24 Fully developed flow boundary condition #1 New Member   Jitender Singh Yadav Join Date: Jul 2009 Location: Pune (India) Posts: 11 Rep Power: 9 I am working on Jets in Crossflow (JICF) problem as a part of my Masters thesis. At a face, which is inlet for the jet, I want to implement "A FULLY DEVELOPED FLOW" condition, that will help saving my length of the jet pipe, otherwise I will have to work on : L(entrance) = 0.06 * Re * D. (for laminar flow) To avoid this, I want to implement such a condition. How I can implement such a condition in OpenFOAM. Thanks a lot.

 December 31, 2009, 01:51 #2 Member   Alan Russell Join Date: Aug 2009 Location: Boise, Idaho USA Posts: 61 Rep Power: 9 jits, One method is to set up the inlet profile with your fully developed flow. The /incompressible/simpleFoam/pitzDailyExptInlet tutorial shows how to do this. There is a file called /constant/boundaryData/inlet/points that has a list of points where you will set your profile. The file /constant/boundaryData/inlet/0/U is where you store the velocity (and other) values for each point. I put the formula in a spreadsheet, calculate the velocity profile data and copy it to the Foam file - this method is working well for me. Good luck, Alan

 January 4, 2010, 00:57 #3 New Member   Jitender Singh Yadav Join Date: Jul 2009 Location: Pune (India) Posts: 11 Rep Power: 9 thanks AlanR, i shall surely try this , seems this should work, even if its 3d I flow, I hope the same things should hold. thanks once again.

 January 4, 2010, 05:43 #4 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,713 Rep Power: 27 Hi Jitender Another approach is to look in the example ~/OpenFOAM/OpenFOAM-1.6.x/tutorials/incompressible/pisoFoam/les/pitzDailyDirectMapped where a mapping procedure is carried out between to planes with a given offset between them. The profile from the interior plane is mapped back on to the inlet, hence between these two planes you basically have an infinitely long pipe, and since you are considering laminar flows, then the distance between the two planes is of minor importance as far as the validity of the velocity (and turbulence) profile(s) goes. I have some nice pictures of a laminar jet in a laminar cross flow on which I performed a POD-analysis, so if you are interested in seeing the results just drop me an email. Happy New Year, Niels Mojtaba.a, sunliming, arvindpj and 3 others like this.

 January 4, 2010, 06:10 #5 New Member   Jitender Singh Yadav Join Date: Jul 2009 Location: Pune (India) Posts: 11 Rep Power: 9 thanks a lot and i wish the same for you. i viewed the pitzDailyMapped case, but i couldn't find out at what offset the values are mapped. and how many times the values are mapped. Are they mapped untill the flow becomes fully developed. thanks

 January 4, 2010, 06:52 #6 Senior Member   Niels Gjoel Jacobsen Join Date: Mar 2009 Location: Deltares, Delft, The Netherlands Posts: 1,713 Rep Power: 27 Hi Look at the following file in the tutorial case: "system/changeDictionaryDict". Running the utility changeDictionary before running the application changes the boundary type in constant/polyMesh/boundary with whatever is stated in the first file. In the first file you also state the offset vector of the given patch. I will send you an email later today with my results. Bests, Niels Asgarian likes this.

 September 8, 2011, 11:29 Hi #7 New Member   Ali Asgarian Join Date: Jul 2011 Location: Toronto, CA Posts: 4 Rep Power: 7 Hi, I guess this page was active long before, but it is still worthy to ask my question. I need to simulate fully developed flow in a geometry (e.g. pipe) with one inlet and one outlet. I prefer to avoid modelling a long pipe; can I implement the same method to model small piece of pipe instead? Tanx

November 2, 2011, 17:10
#8
New Member

Naser Imran Hossain
Join Date: Sep 2011
Posts: 6
Rep Power: 7
Quote:
 Originally Posted by jits_aps90 I am working on Jets in Crossflow (JICF) problem as a part of my Masters thesis. At a face, which is inlet for the jet, I want to implement "A FULLY DEVELOPED FLOW" condition, that will help saving my length of the jet pipe, otherwise I will have to work on : L(entrance) = 0.06 * Re * D. (for laminar flow) To avoid this, I want to implement such a condition. How I can implement such a condition in OpenFOAM. Thanks a lot.
Hey, do you have any idea how to do that in FLUENT? I'm having the same problem where I need a fully developed flow at the inlet but don't want to change the pipe length. Some help would be really appreciated.

 Tags boundary condition, fully developed flow.

 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 durga Main CFD Forum 0 December 8, 2009 01:42 Usman CFX 12 December 20, 2007 12:26 JAS FLUENT 4 February 12, 2007 07:01 Twiti CFX 1 January 24, 2005 02:31 ram Main CFD Forum 5 June 17, 2000 21:31

All times are GMT -4. The time now is 22:55.

 Contact Us - CFD Online - Top