# Uz velocity in 2D

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

 June 12, 2007, 03:49 Hello Im computing an airfo #1 hoochie Guest   Posts: n/a Hello Im computing an airfoil in some cases in 2D. Im interested in the values for lift- and dragforces with second order for my diploma work. I always got a strange velocity in z-direction, which made no sense. I tried all options I have, to solve this problem, but with no success. So I tried to run one tutorial ( pitzdaily ) in second order and discovered in the results a velocity in z-direction too. The look of this z-velocity in paraFoam is similar to my z-velocities in the case of my airfoil. By the way, computing the pitzDaily-case in first order with upwind, produceses no z-velocity. For detailed information please look into my topic: "Uz-velocity in 2D" in the "Running / Solving / CFD"-section of this forum Thx in advance RW

 June 12, 2007, 04:03 If the accumulation of discret #2 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 13 If the accumulation of discretisation/round-off errors and/or round-off errors in the mesh are causing in 2D cases either the problematic component of the velocity should be explicitly removed or the empty mesh patches converted into symmetry planes in order to constrain the spurious flow in the undefined direction. Henry

 June 12, 2007, 04:35 Hello Henry, thank you for #3 hoochie Guest   Posts: n/a Hello Henry, thank you for your reply. In my airfoilcases I changed the boundary conditions for front- and backplane already to symmetryPlane in hope to fix this problem, but even in this I get a velocity in z-direction. This z-velocity is not that high as it is in empty, but it is increasing iteration by iteration. So after xxx iterations, it may have the same value as in the empty-boundary. If I got front- and backplane in "symmetryPlane", Uz is not converging, this may destroy my whole computation. So my values for lift and drag are flipping around. RW

 June 12, 2007, 04:49 I am getting really bored list #4 Senior Member   Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,762 Rep Power: 21 I am getting really bored listening about this week after week - could you please pack up the case, I'll run it here and tell you precisely what's wrong. Hrv __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

 June 12, 2007, 04:54 Edit: About removing the prob #5 hoochie Guest   Posts: n/a Edit: About removing the problematic component: Is there a easy way to patch Uz to 0 in the whole computation for example, or do I have to update some code in the solver? Anyway, if there is no velocity in z, why does OpenFoam computes a velocity in z-direction? All Im interested in is the lift- and dragforce, but with this Uz- problem, it is hard to evalute the results. I dont know in how far the wrong Uz will have an effect on my results. RW

 June 12, 2007, 04:59 Hello Hrv, thank you for yo #6 hoochie Guest   Posts: n/a Hello Hrv, thank you for your reply and your help. Its not my intention to disturb you the whole time, but as it is a mainpart of my diploma work, I would really appreciate a solution. I hope you understand this. Is it ok, if I mail my case to you? RW

 June 12, 2007, 05:11 To remove the z-component of v #7 Senior Member   Join Date: Mar 2009 Posts: 854 Rep Power: 13 To remove the z-component of velocity a quick hack is to add U.replace(vector::Z, 0.0*U.component(vector::Z)); after the velocity corrector in the PISO loop. Henry

 June 12, 2007, 05:19 Hello Henry, thank you very #8 hoochie Guest   Posts: n/a Hello Henry, thank you very much. RW

 June 12, 2007, 05:51 Hello Henry Weller, it look #9 hoochie Guest   Posts: n/a Hello Henry Weller, it looks like removing the z-component did the trick. My residuals look good now, my lift- and dragforces converge to a value, in the past they flipped around, the pictures in paraFoam in case of pressure, Ux and Uy look good. Looks like I can work with the results. So, thank you very much RW

 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 anita OpenFOAM Running, Solving & CFD 7 September 25, 2012 05:35 kees FLUENT 3 April 16, 2008 18:35 KEES Main CFD Forum 0 April 15, 2008 11:26 jrg Main CFD Forum 1 November 19, 2007 14:09 nash Main CFD Forum 0 October 18, 2006 16:37

All times are GMT -4. The time now is 03:29.