CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Post-Processing (http://www.cfd-online.com/Forums/openfoam-post-processing/)
-   -   foamToVTK ERROR, help me! (http://www.cfd-online.com/Forums/openfoam-post-processing/107570-foamtovtk-error-help-me.html)

Bombolati October 1, 2012 11:53

foamToVTK ERROR, help me!
 
Hi at all!
I've done a simulation with reactingFoam. Now I've a folder for every writing point that is fixed in the controlDict file. The next step is postprocess the case with paraFoam but I'm working in a parallel environment and there is only paraview installed. So I thought to use the foamToVTK utility to visualize the case with paraview. When I run this utility this error encountered:

--> FOAM FATAL ERROR:
More than one patch accessing the same transform but not of the same sign.
patch:CameraFL1_shadow transform:0 sign:-1 current transforms ( -1 0 0)

From function Foam::label Foam::globalIndexAndTransform::addToTransformIndex
(
const label,
const label,
const bool
) const

in file lnInclude/globalIndexAndTransformI.H at line 240.

FOAM exiting


I've done the mesh in gambit ad I've exported it with fluent3DMeshToFoam utility. The mesh has some surfaces defined as cyclic, CameraFL1_shadow is one of this.
Someone know how this error encountered?
Thanks a lot.

wyldckat October 1, 2012 17:21

Greetings Bombolati,

I'm not sure at which level you're doing parallel processing, but if in the cluster you can load the whole case in a single machine for post-processing, then you could use ParaView's internal ".foam" reader. Run this command inside your case folder:
Code:

touch case.foam
Then open the "case.foam" file in ParaView. You then have a choice to load either the reconstructed or parallel case.

As for the problem with foamToVTK: did you check the mesh before running the case?
Code:

checkMesh -constant
Best regards,
Bruno

Bombolati October 2, 2012 04:38

Hi Bruno and thanks a lot for you answer. I used the first command to create the file <<case.foam>> and all is ok. Next I tried to use the utility <<check mesh>> and some problems come out. I post here below the result:

Create time

Create polyMesh for time = constant

Time = constant

Mesh stats
points: 1527113
faces: 17663239
internal faces: 17406505
cells: 8766526
boundary patches: 20
point zones: 0
face zones: 4
cell zones: 1

Overall number of cells of each type:
hexahedra: 0
prisms: 0
wedges: 0
pyramids: 3640
tet wedges: 0
tetrahedra: 8762886
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface topology
CameraFL2_shadow 9308 4792 ok (non-closed singly connected)
CameraFL2 9308 4792 ok (non-closed singly connected)
CameraFL1_shadow 19082 9725 ok (non-closed singly connected)
CameraFL1 19082 9725 ok (non-closed singly connected)
MixerFL_shadow 1820 1908 ok (non-closed singly connected)
MixerFL 1820 1908 ok (non-closed singly connected)
IniettoreAriaFL_shadow15463 7907 ok (non-closed singly connected)
IniettoreAriaFL 15463 7907 ok (non-closed singly connected)
CameraFSup 40844 20654 ok (non-closed singly connected)
IngAria 12544 6427 ok (non-closed singly connected)
CombIng2 1684 891 ok (non-closed singly connected)
CombIng1 1682 890 ok (non-closed singly connected)
CameraFL 10446 5408 ok (non-closed singly connected)
MixerFint 7254 3817 ok (non-closed singly connected)
MixerFext 11222 5788 ok (non-closed singly connected)
IniettoreAriaFint 12196 6261 ok (non-closed singly connected)
TestaPiano 1959 1040 ok (non-closed singly connected)
IniettoreAriaFext 36654 18584 ok (non-closed singly connected)
Bordo 12707 6474 ok (non-closed singly connected)
CameraFinf 16196 8269 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-1.29063e-15 -2.17066e-14 -7.10543e-15) (98 98 57)
Mesh (non-empty, non-wedge) directions (1 1 1)
Mesh (non-empty) directions (1 1 1)
Boundary openness (-3.55779e-15 -4.11417e-15 2.20632e-15) OK.
Max cell openness = 3.30458e-16 OK.
Max aspect ratio = 8.87394 OK.
Minumum face area = 0.00211186. Maximum face area = 1.39301. Face area magnitudes OK.
Min volume = 5.43598e-05. Max volume = 0.441604. Total volume = 231604. Cell volumes OK.
Mesh non-orthogonality Max: 67.2498 average: 19.7284
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.954274 OK.
**Error in coupled point location: 45673 faces have their 0th vertex not opposite their coupled equivalent. Average mismatch 38.8115.
<<Writing 45673 faces with incorrectly matched 0th vertex to set coupledFaces

Failed 1 mesh checks.

End

What do you think?

wyldckat October 2, 2012 15:58

Hi Bombolati,

Quote:

Originally Posted by Bombolati (Post 384470)
**Error in coupled point location: 45673 faces have their 0th vertex not opposite their coupled equivalent. Average mismatch 38.8115.
<<Writing 45673 faces with incorrectly matched 0th vertex to set coupledFaces

That is enough proof for me to conclude that this is the reason why foamToVTK is complaining!

You'll find a usage example for fluent3DMeshToFoam: http://openfoamwiki.net/index.php/Fl...y_step_example
As you can see, in that example it also indicates that you should check the mesh after conversion ;)

I'm not familiar with fluent3DMeshToFoam, so my advice is to look in the forum for the keywords:
Code:

fluent3DMeshToFoam cyclic
I'm guessing there is a protocol that must be followed for cyclics to be properly converted.

Best regards,
Bruno


All times are GMT -4. The time now is 10:20.