[kandelabr]

Hello.

In an old version of ParaView on Linux there was a checkbox "Include Zones" (also featured in current user's guide: https://cfd.direct/openfoam/user-gui...#x30-2180006.1) but in newer versions it's been replaced with a "Read zones" checkbox.

I haven't been able to deal with cellZones in newer versions at all - they get read but show variables as (partial). What happened or am I doing something the old way but should update?

Thanks!

[kandelabr]

For anyone struggling with the same problem, I got that working:

1. "Zone reader" doesn't work on decomposed cases.
2. writeFormat in controlDict must be ascii (don't know about compression, I don't use it)
3. To convert from binary, change controlDict and use foamFormatConvert
4. Use Extract Block filter in ParaView.

Enjoy and good luck.

[kandelabr]

FYI, the native paraview 5.6 finally does what I want:

• compressed result files (did not test binary)
• decomposed cases
• read zones with a new checkbox "copy data to cell zones"

I can use the native windows PV version with native OF reader just like paraFoam.

[artymk4]

Originally Posted by kandelabr

FYI, the native paraview 5.6 finally does what I want:

• compressed result files (did not test binary)
• decomposed cases
• read zones with a new checkbox "copy data to cell zones"

I can use the native windows PV version with native OF reader just like paraFoam.

I used your instructions for opening foam-extend-4.0 simulation results with native ParaView 5.6.
I need to use native ParaView because if I run command paraFoam, old ParaView 5.4.1 opens up and I have problems with it. I can read zones in 5.4.1 and I can use filter Extract Block and choose cellZones, but all the field data (p, U, T...) is gone. As soon as I tick Read zones, I can't use field data anymore. Like you said, I see fields "p (partial)" instead of p and so on.

I'm want to add a few things to your instructions, maybe it will help someone:
So first you need to create empty file blabla.foam in your case folder. Then run command paraview in Terminal so native ParaView opens. Click Open and select blabla.foam. It is mandatory that you tick internalMesh, Read zones and new option shows up - Copy data to cell zones - tick that too and click Apply. Now you can use filter Extract Block and choose cellZones.