Paraview: Cell data and Point Data?
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?
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
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 :) )
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
|All times are GMT -4. The time now is 00:54.|