CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Main CFD Forum

help with wall functions

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 24, 2010, 17:55
Default help with wall functions
  #1
New Member
 
Join Date: Jun 2009
Posts: 27
Rep Power: 8
dshawul is on a distinguished road
hello.
I am trying to implement k-e model with wall functions. Model equations are solved alright but I am having difficulty how to go on with wall functions.
Versteeg (eq.3.39) gives equations for u+, k and e to be used close to walls when 30 < y+ < 300. My questions are
a) Do I apply k & e close to wall as Dirichlet bc with those formulas?
b) Do I apply the log-law for all cells which fall in the range of the log law ? what if a boundary cell is equally adjacent to two walls ? Or i use unstructured mesh.
c) Are wall functions necessary for the k-e model ? Because right now it can solve some problems with relatively low Re number but diverges when i go over 10^4. If i avoid solving k&e it goes much more higher, but obviously to the wrong solution.
Thanks in advance for any hints
Daniel
dshawul is offline   Reply With Quote

Old   September 25, 2010, 00:41
Default
  #2
Senior Member
 
Hamid Zoka
Join Date: Nov 2009
Posts: 162
Rep Power: 8
Hamidzoka is on a distinguished road
it should be noted that turbilence models like k-e are devided into two groups from view point of near wall treatment: 1-high reynolds numbers 2-low raynolds number models. when you are concerned will high reynolds ones you should make these modifications(i.e. application of wall function) only to wall adjacent cells. not all the cells lying in range of 30 to 300. in this case the width of wall adjacent cell will be selected such that its y+ lies in the range named above.
generally speaking, concept of y+ is only meaningful in wall adjacent cells.
on the other hand, low reynolds models does not need any wall function.but cells width in near wall region should selected such that Y+ falls well below 10 for adjacent mesh and this increases number of meshes and consequently the run time.
then firstly, you should select your turbulence model.
if you use standard k-e model, be informed that this model is a high reynolds number one.
you can refer to UMIST university .pdf files about wall functions and their application. it can be easily found in internet.
Hamidzoka is offline   Reply With Quote

Old   September 25, 2010, 07:56
Default
  #3
New Member
 
Join Date: Jun 2009
Posts: 27
Rep Power: 8
dshawul is on a distinguished road
Thank you very much for taking the time to reply.
I wrongly thought that for standard k-e ( high Re model), I could avoid
using wall functions as long as i use very fine mesh near walls.
But I now understand the model coefficients are correct only with the use of
wall functions.
thanks again. I am on to googling the UMIST publications.
dshawul is offline   Reply With Quote

Old   September 27, 2010, 08:52
Default Wall functions Turbulence Model
  #4
Member
 
Hans Bihs
Join Date: Jun 2009
Location: Trondheim, Norway
Posts: 34
Rep Power: 8
valgrinda is on a distinguished road
Hei,

to answer you question a):
1) Explicit Time Discretization:
-k: add the whole wall function term to the source term
-e: Dirichlet BC

1) Implicit Time Discretization:
-k: split the wall function term, the part which includes k goes to the ap coefficient, the rest into the source term
-e: either Dirichlet BC or add -10^{30} to the ap coefficient and multiply the wall function term with 10^{30} and add it to the source term

Cheers
Hans
valgrinda is offline   Reply With Quote

Old   September 27, 2010, 13:51
Default
  #5
New Member
 
Join Date: Jun 2009
Posts: 27
Rep Power: 8
dshawul is on a distinguished road
Dear Hans,
Thank you for the hint. I have found a detailed discussion of wall boundary condition treatment in a late chapter of versteeg, basically same as what you mentioned here. One minor doubt i have is about the use of 10^30 which is larger than (1 / Machine epsilon) ? I will use 10 ^ 15 instead to avoid truncation errors.
regards,
dshawul is offline   Reply With Quote

Old   September 28, 2010, 21:26
Default
  #6
New Member
 
Join Date: Jun 2009
Posts: 27
Rep Power: 8
dshawul is on a distinguished road
Looks like 10^30 is ok as the largest double precision number is 10 ^ 307.
Anyway now everything is working fine except that I do not have something to compare my results to.
I took the source term linearization for the k-e model from here http://staffweb.cms.gre.ac.uk/~ct02/research/thesis/node54.html#eq4:24
phoenics's I suppose. I am using the third one. I was able to linearize the k-source term using Picard's method and get same results when the Cd = 2.
I suppose this parameter is tunable, am I correct ?
But using the same method for the epsilon source term linearization gives me something completely different.
My result looks more like the one given for method 2 ?? Can anyone enlighten me on how the linearization is done ?

regards,
dshawul is offline   Reply With Quote

Old   May 23, 2011, 03:12
Default
  #7
Member
 
jk
Join Date: Jun 2009
Posts: 64
Rep Power: 8
jyothishkumar is on a distinguished road
Dear Mr Daniel,

I have cfd code for laminar flow (channel flow) with colocated grid arrangement. I have implemented k epsilon turbulence model in to this. Now if i see my velocity profile (coming as expected) i found that it is more peakier than that of a laminar profile. Also the pressure at the inlet increasing like anything.

My boundary conditions : Velocity inlet, pressure outlet and wall (top and bottom).

And I have followed the book versteeg and malalasekara. Also I have compared my laminar flow results with FLUENT code and found it is matching but i am getting this peculiar problem for turbulent flow. Please tell me your valuable suggestion.

thanks in advance

jyothish
jyothishkumar is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug unoder OpenFOAM Installation 11 January 30, 2008 21:30
Wall functions tutlhino OpenFOAM Pre-Processing 0 July 2, 2007 05:04
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12
When I use the wall functions....! maximus Main CFD Forum 7 January 20, 2003 10:35
help with wall functions Nick Georgiadis Main CFD Forum 4 February 20, 2000 18:07


All times are GMT -4. The time now is 01:31.