# StreamFunction

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

 July 2, 2013, 10:00 StreamFunction #1 New Member   Luis Batista Join Date: Mar 2013 Location: Lisboa / Setúbal Posts: 17 Rep Power: 5 Hello Forum, I am doing an analysis to a cavity flow using SimpleFoam.... Is there any known issue/error with the OF(2.1.2) function StreamFunction ? Apparently, I am having proper results within my vorticity vector field but when I plot the point field resulting from the streamFunction in Paraview, it seems that the results are 10 times smaller....I also see that the units of the streamfunction scalar field are L3 T-1. How are these units being derived? Regards, Luis

 July 7, 2013, 05:57 #2 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 9,736 Blog Entries: 39 Rep Power: 103 Hi Luis, Can you provide a simple test case? Best regards, Bruno __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide What am I doing/planning: blog/wiki Read this before sending me PM

August 19, 2013, 13:37
#3
New Member

Christiane Lechner
Join Date: Jul 2011
Location: Vienna
Posts: 4
Rep Power: 7
Dear Bruno and Luis,

I find the same with version 1.6-ext: the stream function seems to be too small by a factor of 10 and has dimensions length^3/time.

I attach a case of a linear shear flow, U = (y/H)*V, with H the height of the domain, and V the velocity at the upper boundary.

The stream function should be: \Psi = 0.5*((y/H)^2 -1)*V*H

best regards,
Christiane
Attached Files
 testStreamFunction.tar.gz (25.7 KB, 11 views)

 August 20, 2013, 05:34 #4 New Member   Christiane Lechner Join Date: Jul 2011 Location: Vienna Posts: 4 Rep Power: 7 Hi, the factor 0.1 seems to stem from the cell width in the empty direction, which is \Delta z = 0.1 in the above example. Reducing \Delta z to 0.01 also reduces the streamFunction by another factor of 10. So it seems, that the streamFunction utility computes \Psi*\Delta z, not \Psi. This would also explain the dimensions length^3/time. Do you agree? best regards, Christiane

 August 21, 2013, 09:32 #5 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 9,736 Blog Entries: 39 Rep Power: 103 Greetings Christiane, Many thanks for the test case, but I haven't yet managed to look into it. But I've taken a quick look into the source code of "streamFunction" on both 2.2.x and 1.6-ext: And both calculations seem to be done in the same. I can't find any indication of an explicit scaling factor, which leads me to believe that the phi field that OpenFOAM is using already includes the scale of each cell or face. Because the sign function only gives us "+1" or "-1". Another indication is that it doesn't seem to work for 3D simulations, because it assumes that Z is the empty orientation. I'll try to look at the test case later today. Best regards, Bruno __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide What am I doing/planning: blog/wiki Read this before sending me PM

 August 22, 2013, 12:28 #6 New Member   Christiane Lechner Join Date: Jul 2011 Location: Vienna Posts: 4 Rep Power: 7 Hi Bruno, yes, the face flux field phi is phi = U_f & S_f, with S_f the area of the face. For the computation of the stream function U_f & S_f/\Delta z would be needed instead. best regards, Christiane

 August 22, 2013, 12:59 #7 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 9,736 Blog Entries: 39 Rep Power: 103 Hi Christiane, Of course! Why didn't I visualize that... the face area still depends on Z, even though the flow is only over X-Y. OK, then there are 2 immediate solutions: Use 1.0 for the width of the empty direction, in order to avoid the distortion of the "phi" and "psi" calculation.This reminds me of a 2D tutorial in OpenFOAM that uses the thickness of 1.0m and I didn't understand why... until now. The tutorial is the "combustion/XiFoam/ras/moriyoshiHomogeneous". Request a bug fix for this at the respective bug trackers:Official OpenFOAM: http://www.openfoam.org/bugs/ Extend Project's bug tracker: http://sourceforge.net/apps/mantisbt/openfoam-extend/ Best regards, Bruno __________________ OpenFOAM: FAQ | Getting started Forum: How to get help, to post code/output and forum guide What am I doing/planning: blog/wiki Read this before sending me PM

 August 26, 2013, 04:29 #8 New Member   Christiane Lechner Join Date: Jul 2011 Location: Vienna Posts: 4 Rep Power: 7 Hi Bruno, thanks! I requested bug fixes at both sites: http://www.openfoam.org/mantisbt/view.php?id=976 http://sourceforge.net/apps/mantisbt...iew.php?id=185 best regards, Christiane

 Tags streamfunction

 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 jignesh_thaker2007 OpenFOAM 4 September 29, 2011 12:25 titio OpenFOAM Post-Processing 0 May 19, 2010 16:04 nisha Fluent UDF and Scheme Programming 0 September 15, 2009 06:55 ryoga Main CFD Forum 0 February 1, 2002 19:20 Steven Main CFD Forum 1 December 30, 2000 13:04

All times are GMT -4. The time now is 06:45.