[immortality]

Hi
have anyone tested that reconstructPar time does vanishes parallel processing benefits over serial run time on a local PC(with several threads) or not(parallel processing is better despite of reconstructPar time consumption)?
has done anyone any tests or have any idea?

[ngj]

Hi Ehsan,

The key point probably is that you do not need to reconstruct your results. paraFoam/paraView works on your decomposed case and your post-processing merely need to consider the fact that data is decomposed, once you work with them.

Previously, I also experienced that the reconstruction part took a lot of time, so I have not been doing that for a long time.

Kind regards

Niels

[immortality]

Hi Niels
really there is no need to reconstructPar? I didn't know that! I'll test it,thank you so much.

[cfdonline2mohsen]

Dear Ehsan
In most of the cases you do not need to reconstructPar all the time steps but only the results for the latestTime by using:

reconstructPar -latestTime

which does not take a lot of time.
and reconstructPar is definately required for postprocessing the results using Tecplot.

Dear Niels

The key point probably is that you do not need to reconstruct your results. paraFoam/paraView works on your decomposed case

I remember that in the previous versions of Paraview when I did not reconstructPar my results, it did not show my whole geometry but only my decomposed geometries seperately! (in the processor0 , processor1 ... folders)
does it show your whole geometry or only your decomposed geometry separately?

[ngj]

Hi Kia,

In your ParaView (my version: 3.98.1), there is a drop-down menu just below the "Refresh" bottom. I you change it from "Reconstructed Case" to "Decomposed Case", ParaView gathers the needed decomposed data by itself. It is no longer needed to manually load all N processor directories.

Kind regards

Niels

[immortality]

thanks Mohsen and Niels
I use 3.12.0 and think there is not such an option.and my case is unsteady then I need all time steps.never mind it's not a big issue!

[kwardle]

How are you starting ParaView? If via paraFoam, then use the -builtin flag to use the parallel-aware reader in ParaView. If you are starting paraview on your own from the commandline or otherwise, if you make the controlDict softlink extension ".foam" (instead of .OpenFOAM) it will automatically use the built-in reader which will have the option to select reconstructed or decompose data sets. The "Refresh" button is not in 3.12 but is found in more recent versions (I have 4.0.1), but you could also record a python macro which switches from decomposed to reconstructed and back and this will refresh the times also.

[immortality]

Hi Kent
that was very useful. -builtin option was excellent! thanks.
@Mohsen:
Hi Mohsen

and reconstructPar is definately required for postprocessing the results using Tecplot.

for what type of postProcessing we may need tecPlot on top of paraView?and whats equivalent to tecPlot in ubuntu?

[cfdonline2mohsen]

for what type of postProcessing we may need tecPlot on top of paraView?

Well, actually I have used Tecplot from my B.Sc to PhD for more than 10 years and it's really hard to move to paraView completely and put all the experiences in using Tecplot into the trash can!
we have a proverb for that in Persian that says "old habits die hard"
I am really glad that Tecplot started to support OpenFoam directly without requiring any tools to convert the OF data.

whats equivalent to tecPlot in ubuntu?

Actually there is tecplot-360 for ubuntu.find more information in here:
http://www.tecplot.com/products/tecplot-360/ in requirements section.
and of course it is not free like ParaView!