CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Paraview & paraFoam

Paraview: Cell data and Point Data?

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

Like Tree1Likes
  • 1 Post By sushant

Reply
 
LinkBack Thread Tools Display Modes
Old   July 9, 2010, 10:47
Default Paraview: Cell data and Point Data?
  #1
New Member
 
Vitor Braga
Join Date: Oct 2009
Posts: 28
Rep Power: 7
vitor is on a distinguished road
Hi,

I'm trying to calculate the average velocity in the outlet of a pipe.
I use the filter Integrate Variables, but I dont know how to interpret the data, I mean, what is the difference between the values of velocity in the Cell Data and Point Data? They are quite different.
If I wish to calculate the average velocity in the outlet, which should I choose?
Just to make sure, Paraview integrates in the area, so all I have to do is divide this value by the area of the pipe, and this will give me the average velocity, right?

Thank you.

BR,


Vitor.
vitor is offline   Reply With Quote

Old   July 9, 2010, 13:46
Default
  #2
Senior Member
 
Nima Sam
Join Date: Sep 2009
Location: Tehran, Iran
Posts: 1,075
Blog Entries: 1
Rep Power: 14
nimasam is on a distinguished road
Send a message via Yahoo to nimasam
hi friend
as i guess cell data is the value of cell center but point data are the value of cell points for example in hex mesh we have 8 data for points of a cell but just one data for cell center
nimasam is offline   Reply With Quote

Old   July 10, 2010, 06:30
Default
  #3
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,888
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Quote:
Originally Posted by vitor View Post
Hi,

I'm trying to calculate the average velocity in the outlet of a pipe.
I use the filter Integrate Variables, but I dont know how to interpret the data, I mean, what is the difference between the values of velocity in the Cell Data and Point Data? They are quite different.
The cell values are the raw data saved by the solver, while the point values are interpolated on the cell points.

Quote:
If I wish to calculate the average velocity in the outlet, which should I choose?
If with outlet you mean a boundary condition, the most appropriate way is to average in the code, using the face values on the patch.

Best,
__________________
Alberto

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
GeekoCFD 32bit - The 32bit edition of GeekoCFD.
GeekoCFD text mode - A smaller version of GeekoCFD, text-mode only, with only OpenFOAM. Available in a variety of virtual formats.
alberto is offline   Reply With Quote

Old   December 23, 2010, 01:09
Default Utilities
  #4
Member
 
sushant's Avatar
 
Join Date: Mar 2009
Location: Switzerland
Posts: 42
Rep Power: 7
sushant is on a distinguished road
Take a look at the following utilities:

patchAverage Calculates the average of the specified field over the specified patch
patchIntegrate Calculates the integral of the specified field over the specified patch

If all you want to do is calculate average velocity magnitude over the outlet patch. You don't need to open up ParaView to do that. Note that velocity is a volVectorField and only volScalarFields can be averaged, so use

foamCalc mag U

to find and write magU if you want to work with velocity. Then

patchAverage magU outlet

Quote:
what is the difference between the values of velocity in the Cell Data and Point Data?
From OpenFOAM-Wiki:
The builtin cell-to-point filter works like a Cell Data to Point Data filter in ParaView in that it just takes the average of cell values connected to a point. The difference is that the builtin filter takes boundary patch values into account. The filter is faster but less accurate than the volPoint interpolator in paraFoam, which further does inverse distance weighting of cell values. The cell-to-point filter is still computationally demanding thus can be turned off by unchecking "Create cell-to-point filtered data" on the reader panel.


Quote:
Just to make sure, Paraview integrates in the area, so all I have to do is divide this value by the area of the pipe, and this will give me the average velocity, right?
( ∫∫ ψ dA ) / ( ∫∫ dA )
= ( ∫∫ ψ dA ) / A
= average of ψ over A
So yes.

( Sorry to bump an old thread but hope this is helpful )
sharonyue likes this.

Last edited by sushant; December 23, 2010 at 02:24. Reason: didn't notice OP specifically asked about ParaView
sushant 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
How to get the data of second cell or point near the wall? jelon STAR-CCM+ 0 April 24, 2010 03:04
Velocity vector data in OpenFOAM and ParaView mismatch tekky OpenFOAM 9 December 21, 2009 12:26
Cell Data to Point Data Issues mcintoshjamie OpenFOAM Paraview & paraFoam 2 November 19, 2009 04:55
IFStream read float point data problem liu OpenFOAM Running, Solving & CFD 0 October 24, 2008 13:14
How to update polyPatchbs localPoints liu OpenFOAM Running, Solving & CFD 6 December 30, 2005 18:27


All times are GMT -4. The time now is 21:18.