# turbulent kinetic energy is not zero at the wall

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

 January 29, 2013, 00:25 turbulent kinetic energy is not zero at the wall #1 New Member   yogendra poul Join Date: Sep 2011 Posts: 4 Rep Power: 6 hi all i am solving multiphase turbulent flow problem. velocity profile is correct but turbulent kinetic energy and intensity is not zero at the wall, although it should be zero at the wall. turbulent kinetic energy and intensity is showing maximum on the wall. i do not why is it so? i need help thank you

 January 29, 2013, 03:14 #2 New Member   yogendra poul Join Date: Sep 2011 Posts: 4 Rep Power: 6 i am waiting for guidance from experts. it will really help me a lot.

 January 29, 2013, 05:07 #3 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,118 Rep Power: 19 What kind of wall modeling are you using? If you are using a wall function with Y+ around 60 it is normal that the TKE has a maximum value in the first cell away from the wall. If I recall correctly, the maximum for TKE is occurs at around Y+=30 for a flat plate.

 January 29, 2013, 08:04 #4 New Member   yogendra poul Join Date: Sep 2011 Posts: 4 Rep Power: 6 Thank for your guidance In my case fluid is flowing in a circular pipe. i am using k-omega viscous model. As you told wall model and Y+ value, i am not clear how and where to use wall model and Y+ value. i mean where is the input for Y+ value in gui. probably you are getting my point thank you very much

 January 29, 2013, 12:26 #5 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,118 Rep Power: 19 Y+ is not an input parameter. It is the non-dimensional wall distance of the first cell. You can evaluate it as a post-processing variable at solid walls. The only way to influence it (besides the flow conditions) is with the mesh size. If you want to resolve the boundary layer and thus capture the "correct" behavior of the flow variables near the wall, Y+ should be around 1 as a rule of thumb. Additionally, you will have to use the "enhanced wall treatment" in the turbulence modeling section.

 January 30, 2013, 07:00 #6 New Member   yogendra poul Join Date: Sep 2011 Posts: 4 Rep Power: 6 thank you very much Alex S

 January 30, 2013, 10:47 #7 New Member   Matty Join Date: Nov 2011 Posts: 5 Rep Power: 5 It may help to use the scalable wall treatment if it is available with the turbulence model you are using. This applies the different wall treatments based on the value of Y+ or Y* as far as i am aware. I had this problem as well a while ago. Good luck.

April 28, 2014, 11:03
#8
Member

Sheng
Join Date: Jun 2011
Posts: 58
Rep Power: 6
Quote:
 Originally Posted by yogi06_sati hi all i am solving multiphase turbulent flow problem. velocity profile is correct but turbulent kinetic energy and intensity is not zero at the wall, although it should be zero at the wall. turbulent kinetic energy and intensity is showing maximum on the wall. i do not why is it so? i need help thank you
Hi guys,
I think the question is to ask why turbulent kinetic energy and turbulence intensity are not zero at the wall, but the replies are all related to Y-plus!

The answer is, FLUENT doesn't implement zero boundary condition for kinetic energy k (k omega based model)! It uses zero gradient boundary condition (the change rate across the wall boundary is zero, instead of fixing a zero value for k), so you will see a finite value of k on the wall. I don't know why FLUENT does this. Among literature, I see some use zero, while some use zero gradient. You probably need a reference discussing boundary condition. The k change very near wall surface may be quite not trustful. One guy from my university shows me the difference from FLUENT and in-house DNS code. He then implements a UDF turbulence model using zero value boundary condition and also finds difference from FLUENT default turbulence models.

Sheng

 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 alanlove FLUENT 1 November 23, 2012 12:24 unoder OpenFOAM Installation 11 January 30, 2008 21:30 ph FLUENT 1 January 31, 2007 09:55 MET FLUENT 8 December 8, 2006 06:08 Meri CFX 0 February 22, 2005 07:00

All times are GMT -4. The time now is 05:20.

 Contact Us - CFD Online - Top