Error using foamToVTK in the newest CFDEM 3.8.0

Submitted by Rachel on Thu, 12/07/2017 - 20:58

Dear all,

I have just installed the newest version of CFDEM (3.8.0) and have sucessfully run the example case in my computer (i.e ErgunTestMPI). However when I am trying to transfer the CFD results into VTK files, I use the command "foamToVTK" and get the error message as below:

---> FOAM FATAL IO ERROR:
wrong token type - expected scalar, found on line 5 the punctuation token ')'

I didn't change anything of this example and I don't know how to fix this problem, could anyone please give some clues? Thanks ahead!

Regards,
Rachel

Forums:

buaa_rainbow's picture

buaa_rainbow | Mon, 12/11/2017 - 16:30

I encountered the same problem in the packedBedTempParScale example
when i reconstructPar the cfd file
error occurs like this
--> FOAM FATAL IO ERROR:
wrong token type - expected Scalar, found on line 5 the punctuation token ')'

file: /home/hwb/CFDEM/hwb-PUBLIC-5.0/run/tutorials/ParScale/cfdemSolverPisoSTM/packedBedTempParScale/CFD/processor0/0.1/lagrangian/particleCloud/positions at line 5.

From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::doubleScalar&)
in file lnInclude/Scalar.C at line 93.

FOAM exiting

e:buaa_rainbow#buaa.edu.cn

Neiht | Wed, 01/17/2018 - 02:10

Below is actually the format of the 0.../lagragian/positions in OF 5.x:
24750
(
(0.385047 0.507097 0.0772844 0.0305708) 0 16440 2
(0.539439 0.145015 0.0290815 0.286465) 0 13320 2
(0.000100127 0.699197 0.0355707 0.265132) 0 0 1
(0.5319 0.325039 0.0372543 0.105807) 1 13350 2
(0.391212 0.499963 0.0394776 0.0693481) 1 13740 1
(0.19576 0.638586 0.066483 0.0991711) 0 1 1
(0.1966 0.304931 0.161569 0.3369) 0 1 2
(0.000202668 0.0989364 0.648569 0.252292) 0 0 1
(0.192827 0.50163 0.1539 0.151643) 1 3 2
(0.188971 0.103782 0.161031 0.546215) 1 3 2
(0.398723 0.300247 0.0714553 0.229574) 2 16441

The format of .../positions is different.
2494
(
( -0.0108926 -0.00401486 0.00049965 ) 0
( -0.0050677 -0.00114585 0.000997539 ) 0
( -0.00678609 -0.00690088 0.00293997 ) 0
( -0.000965258 -0.00189565 0.00280136 ) 0
( -0.0130612 -0.0024788 0.00049936 ) 0
( -0.00939874 -0.0044298 0.000499396 ) 0
( -0.00305486 -0.00787107 0.0011839 ) 0
( -0.000104195 -0.00572686 0.00455995 ) 0
( -0.00875944 -0.0018514 0.005338 ) 0
...

It still using the old format. I think we need to switch to old version of OF to reconstructure or convert to VTK with the case or use old version of OF instead of 5.x to couple

Cheers,
Thien Phan

Neiht | Wed, 01/17/2018 - 02:16

Hi all,

I worked when I tried to reconstruct and convert to VTK with the OF 4.x ( I have more than one OF version on my ubuntu and switch among them by alias).
Hope you can solve your problem with this solution as well.

Cheers,
Thien Phan

paul | Wed, 01/17/2018 - 22:21

Do reconstructPar -noLagrangian or at least foamToVTK -noLagrangian.
This prevents OF from trying to read the old position-based particle data from the time directories.
CFD data can be easily visualized in ParaView without having to reconstruct using the builtin OF reader:
touch case.foam
paraview case.foam
and selecting case type decomposed.

The output of lagrangian data in the time directories can be disabled in the couplingProperties by setting IOModel -> off.
Particle data is best dumped directly from LIGGGHTS using dump custom/vtk.

- Paul