# Paraview: Cell data and Point Data?

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

 July 9, 2010, 09:47 Paraview: Cell data and Point Data? #1 New Member   Vitor Braga Join Date: Oct 2009 Posts: 28 Rep Power: 10 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.

 July 9, 2010, 12:46 #2 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,240 Blog Entries: 1 Rep Power: 18 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

July 10, 2010, 05:30
#3
Senior Member

Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28
Quote:
 Originally Posted by vitor 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 Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541)
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.

December 23, 2010, 01:09
Utilities
#4
Member

Join Date: Mar 2009
Location: Switzerland
Posts: 40
Rep Power: 10
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 )

Last edited by sushant; December 23, 2010 at 02:24. Reason: didn't notice OP specifically asked about ParaView

 May 15, 2015, 17:56 #5 Member   james wilson Join Date: Aug 2014 Location: Orlando, Fl Posts: 38 Rep Power: 5 I found this relevant thread but didn't find any specific information for my case. I'm looking to access cell point values associated with a field. I'm using a hex mesh and am doing interface reconstruction. I require access to the point values since using cell values alone for calculating the interface normal only considers 6 adjacent cells (2 in x, y and z) for 3D and is less accurate and results in large parasitic currents. Any advice regarding RUNTIME utilities, functions etc. would be beneficial. See also: http://www.cfd-online.com/Forums/ope...ue-access.html James Last edited by jameswilson620; May 27, 2015 at 12:21. Reason: bad link

 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 jelon STAR-CCM+ 0 April 24, 2010 02:04 tekky OpenFOAM 9 December 21, 2009 12:26 mcintoshjamie OpenFOAM Paraview & paraFoam 2 November 19, 2009 04:55 liu OpenFOAM Running, Solving & CFD 0 October 24, 2008 12:14 liu OpenFOAM Running, Solving & CFD 6 December 30, 2005 18:27

All times are GMT -4. The time now is 20:15.