# Definition of y+ in yPlusRAS (1.7.1)

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

 October 17, 2011, 08:48 #21 Senior Member   Join Date: Mar 2009 Posts: 135 Rep Power: 6 I get 0 on every wall for fully resolved boundary layers. As reported here: Problems with YPlusRAS and wallShearStress For wallFunction I get value but I canīt assess them... __________________ OF - 2.0.0

 October 18, 2011, 20:53 y+ = y* #22 New Member   Saxwax Join Date: Aug 2010 Posts: 17 Rep Power: 5 Hi Cameosas, Glad to hear that the file compiled, not sure about the 0 for fully resolved boundary layers. It is possible that I used the old version of Niklas' yPlus utility. Have you checked that? Vaina74, I'm not sure which version of the FLUENT manual you are quoting. In the version that I have (Version 12 April 2009) the section Near-Wall Treatment for Wall Bounded FLows contains the following quote: "It should be noted that, in ANSYS FLUENT, the laws-of-the-wall for mean velocity and temperature are based on the wall unit, y*, rather than y+. These quantities are approximately equal in equilibrium turbulent boundary layers." Comparing the equations for y+ and y* we can see that the only difference between the two are the frictionVelocity, Cmu^0.25 and k^0.5 terms. y+ = rho*frictionVelocity*y/mu y* = rho*(Cmu^0.25)*(k^0.5)*y/mu For equilibrium turbulent boundary layers (ETBL) frictionVelocity = (Cmu^0.25)*(k^0.5) (Ferziger), i.e. y+ is equal to y*. If you are using standard wall functions for flows with an ETBL then y*, or yPlusRAS, probably will give you a good enough indication of the appropriateness of your cell size. Not sure if that helps (it definitely wont if I am wrong ). Let me know your thoughts on this one. It would be good to have a better idea on why things are the way they are in OpenFOAM. Regards, D.

 October 20, 2011, 05:09 #23 Senior Member   Join Date: Mar 2009 Posts: 135 Rep Power: 6 HI Saxwax, I have downloaded both, but I am using the newer version. __________________ OF - 2.0.0

 October 25, 2011, 00:50 Nut? #24 New Member   Saxwax Join Date: Aug 2010 Posts: 17 Rep Power: 5 Cameosas, The way I see it, based on the equation used to calculate the cell y+ value in the yPlus utility there are three possible reasons why a value of exactly zero would be output: 1) y = 0 2) snGrad = 0 3) nut = 0 Two of these are very easy to check, y and nut. The third is also probably quite easy to check (edit yPlus utility to output snGrad instead) - I haven't tried this. My guess would be that nut is the likely culprit. Either a boundary condition at the wall is set to nut = 0, or the wall function being used (i.e. nutkWallFunction) is calculating the nut value at some (or all) points to be zero. I'd either have a look at the nut file or colour the wall patch by nut in Paraview. I have noticed the same zero values being output by yPlus. A quick check showed that the nut field had several cells showing up as zero (nutkWallFunction). I'm not really sure if this is the expected behavior or not. Someone else can probably answer that. Regards, D. Last edited by Saxwax; October 25, 2011 at 02:10.

 October 25, 2011, 11:00 #25 Senior Member   Join Date: Mar 2009 Posts: 135 Rep Power: 6 HI Saxwax, Thats a really good hint! Thanks! I get zero values for: Code: `yPlus.boundaryField()[patchi] = y[patchi]` AND for: Code: `yPlus.boundaryField()[patchi] = mut.boundaryField()[patchi]` (I am using the compressible version) Code: ``` yPlus.boundaryField()[patchi] = mag(U.boundaryField()[patchi].snGrad());``` gives non zero values. in the order of 1e3 Code: ``` yPlus.boundaryField()[patchi] = (RASModel->mu().boundaryField()[patchi]/rho.boundaryField()[patchi]);``` gives non zero values in the order of 1e-5 __________________ OF - 2.0.0 Last edited by camoesas; October 26, 2011 at 02:47.

 October 26, 2011, 04:06 #26 Senior Member   Join Date: Mar 2009 Posts: 135 Rep Power: 6 I have defined the walls for mut like: Code: ``` { type mutkWallFunction; value uniform 0; }``` Thats like its defined in the tutorials... __________________ OF - 2.0.0

 November 1, 2011, 21:11 #27 New Member   Saxwax Join Date: Aug 2010 Posts: 17 Rep Power: 5 Cameosas, Are the zero values for mut and y in the same cells (or all the cells)? If so I would guess that the mutkWallFunction uses y to calculate the mut value. You could check this by looking at the mutkWallFunction.C source code. This way you would know that the zero values originate from y. If not well then I am not really sure. Again, looking at the source code may help. Regards, D.

 June 10, 2013, 04:56 #28 Member   Join Date: Aug 2011 Posts: 47 Rep Power: 4 Hello, I just want to check that yPlusRAS is calculating the right thing. So I calculated yPlus with yPlusRAS and by hand with this equation: yPlus= Cmu^(0.25) * y * k^(0.5) / nu with: Cmu =0.09 y = 0.00125 (it is the cell height / 2 because I am looking at the cell directly at the wall) k = 0.19 (from paraview) nu = 1.0e-6 So i get: yPlus = 298 yPlusRAS says: yPlus = 6.7 The domain is a rectangular channel, so Iīve got a nice grid. To get the yPlus from yPlusRAS I should use y = 2.8e-5 Can somebody help me what is wrong? Thanks a lot

 June 11, 2013, 04:00 #29 Member   Join Date: Aug 2011 Posts: 47 Rep Power: 4 I found my mistake the yPlus = 6.7 was shown in paraview. If I look at the output in the shell after I tipped yPlusRAS I see complete different values in comparison to the values in paraview. But the values in the output are the values I calculated by hand. So the interpolation in paraview was the problem. But still one simple question is left: I have a rectangular channel and I decided to use wall functions for k, epsilon and nut. Am I right that the distance from the wall to the cell centre of the first cell at the wall has to be smaller than yPlus = 11? If itīs not, do I get a wrong result? I am also not sure what k I should use for calculating yPlus. At the beginning I only have the k which I enter in the k-file. But at the end of my simulation the k at the wall has changed. So yPlus has changed too. So maybe after the run I know that my grid should be smaller. How can I solve this problem? thanks a lot for your help

 Tags komegasst, openfoam 1.7.1, simplefoam, yplusras

 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 asaijo OpenFOAM Installation 9 April 6, 2011 13:21 Luiz CFX 4 March 6, 2011 21:02 opencfd OpenFOAM Announcements from ESI-OpenCFD 0 August 26, 2010 12:40 ivan_cozza OpenFOAM Running, Solving & CFD 0 September 23, 2009 06:27 gschaider OpenFOAM Installation 118 July 20, 2008 06:19

All times are GMT -4. The time now is 14:42.