|July 9, 2010, 09:47||
Paraview: Cell data and Point Data?
Join Date: Oct 2009
Posts: 28Rep Power: 9
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?
|July 9, 2010, 12:46||
Join Date: Sep 2009
Location: Tehran, Iran
Blog Entries: 1Rep Power: 16
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||
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910Rep Power: 27
GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats.
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||
Join Date: Mar 2009
Posts: 42Rep Power: 9
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
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.
= ( ∫∫ ψ dA ) / A
= average of ψ over A
( 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||
Join Date: Aug 2014
Location: Orlando, Fl
Posts: 38Rep Power: 4
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: interface reconstruction and point value access
Last edited by jameswilson620; May 27, 2015 at 12:21. Reason: bad link
|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 02:04|
|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 12:14|
|How to update polyPatchbs localPoints||liu||OpenFOAM Running, Solving & CFD||6||December 30, 2005 18:27|