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

y+ distribution (time history)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 4, 2008, 20:14
Default y+ distribution (time history)
  #1
Deloat
Guest
 
Posts: n/a
Hi all,

I am currently modelling a flow past a 3d cylinder, and is required to find the timehistory of y+ distribution. Does anyone know how to find this info?

I tried to plot the 'Yplus', using the contour plots and selecting the cylinder as the location of the plot, but it seem that all other timestep show a Yplus contour plot of 0, while the last timestep shows a variation in contour plots of the Yplus. Any idea why this is happening?

Also, is there a way to ask cfx-solver or cfx-post to find the y+ of the cylinder instead of using contour plots, as i need a numerical value for y+.

Thanks in advance, Deloat
  Reply With Quote

Old   March 4, 2008, 20:30
Default Re: y+ distribution (time history)
  #2
UnderwaterAlex
Guest
 
Posts: n/a
Hi Deloat,

This probably means you did not store the values of y+ at the intermediate steps. That is why the rest of the time (other than the final timestep) it shows up as gray or another solid color. You have to ensure that you have selected it as a variable to keep in your .trn results under Output Control in CFX-Pre. When you load the .res or .bak file, it contains all the results for the final timestep, which is why it is displayed there but nowhere else.

As for a numerical value, you need to think about which one. Do you need the max anywhere on the body at each timestep, or the entire variation on a 2D surface at each timestep? To find just the max, or a value at a particular point, you can use the CEL expressions probe or maxVal in Post and create a time varying chart. To make a single plot that shows the variation with time at each location on a body will require visualization skills far beyond mine.

Best of luck,

-Alex

  Reply With Quote

Old   March 4, 2008, 20:48
Default Re: y+ distribution (time history)
  #3
Deloat
Guest
 
Posts: n/a
Thanks for your reply. I just want to find the max value anywhere on the body. You mentioned about using maxVal in Post, can you explain further?

I dont think i want to write an CEL expression because i am not that familiar with that. I just want an easy way out just so that i can find the max value of y+ on the cylidner, as this step is just a check whether my meshing is sufficient. Can you show me how to do it in Post?

Thanks in advance, Deloat
  Reply With Quote

Old   March 5, 2008, 12:02
Default Re: y+ distribution (time history)
  #4
UnderwaterAlex
Guest
 
Posts: n/a
You can create CEL expressions in Post as well as Pre. Here's how I would find the max y+, assuming you have a set of .trn files that contain the variable y+ at each timestep. (Without that, there is not much to be done.)

In Post, click on the "Quantitative" tab of the top left panel. this will bring up the expressions panel. Right click and choose new, and give it a name like maxyplus. In the expression window, type maxVal(Yplus)@Cylinder (or whatever the surface of the cylinder is called.) Click apply.

Next you do Insert -> Chart, Chart Type change from XY to Time. Under the Chart Line 1 panel, change Method from Point to Expression. In Expression input maxyplus. Click apply again and then refresh the chart if necessary. That should do it.

-Alex
  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
Multiple floating objects CKH OpenFOAM Running, Solving & CFD 12 March 21, 2016 14:05
calculation diverge after continue to run zhajingjing OpenFOAM 0 April 28, 2010 04:35
calculation the residence time distribution by CFX ahmedsalemy CFX 4 June 25, 2009 10:40
Modeling in micron scale using icoFoam m9819348 OpenFOAM Running, Solving & CFD 7 October 27, 2007 00:36
Transient simulation not converging skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48


All times are GMT -4. The time now is 03:14.