CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Paraview & paraFoam (https://www.cfd-online.com/Forums/openfoam-paraview/)
-   -   Paraview: Cell data and Point Data? (https://www.cfd-online.com/Forums/openfoam-paraview/78009-paraview-cell-data-point-data.html)

 vitor July 9, 2010 09:47

Paraview: Cell data and Point Data?

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.

 nimasam July 9, 2010 12:46

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

 alberto July 10, 2010 05:30

Quote:
 Originally Posted by vitor (Post 266595) 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,

 sushant December 23, 2010 01:09

Utilities

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 :) )

 jameswilson620 May 15, 2015 17:56

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.