|
[Sponsors] |
November 4, 2015, 05:56 |
pointIndex = -1 in paraView
|
#1 |
Member
Karelke Yu
Join Date: Dec 2014
Posts: 96
Rep Power: 11 |
dear foamers.
i am now confused by the -1 pointIndex in paraView, as what has been attached. although the polyMesh is generated manually, i firstly do not think this comes from the files in polyMesh folder because it seems that the geometry and topology can be recognized. besides, the pointIndex -1 seems to correspond to the cell type (Pyramid and Tetrahedron). i am very sorry that my mesh files could not be uploaded correctly. could someone give some hints or suggestions with the attached image? thanks a lot! /karelke |
|
December 6, 2015, 15:04 |
|
#2 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
Quick question: How exactly are you getting these arrays named "Point Index *"? Did you use a filter in ParaView to generate these fields?
Because my guess is that these fields were loaded from the time folder, e.g. from the folder "0". |
|
December 8, 2015, 06:11 |
|
#3 | |
Member
Karelke Yu
Join Date: Dec 2014
Posts: 96
Rep Power: 11 |
Quote:
i am working on paraview 4.1.0 and i think i do not use any filter to generate fields. i just want to view the mesh and paraview gives me this strange results. i choose the Spreadsheet View option and change the Attribute from fields to cell data because i just intend to view the mesh. and then i got what shown in the attached image. checkMesh gives: Code:
Checking geometry... Overall domain bounding box (1.12393e+06 -1.69078e+06 -0.5) (1.25165e+06 -1.54424e+06 0.5) Mesh (non-empty, non-wedge) directions (1 1 0) Mesh (non-empty) directions (1 1 0) All edges aligned with or perpendicular to non-empty directions. ***Boundary openness (-0.0010534 -0.00041202 0) possible hole in boundary description. ***Open cells found, max cell openness: 1, number of open cells 2170 <<Writing 2170 non closed cells to set nonClosedCells ***Zero or negative face area detected. Minimum area: 0 <<Writing 6 zero area faces to set zeroAreaFaces ***Zero or negative cell volume detected. Minimum negative volume: -1.90841e+06, Number of negative volume cells: 2155 <<Writing 2155 zero volume cells to set zeroVolumeCells Mesh non-orthogonality Max: 179.997 average: 161.432 *Number of severely non-orthogonal (> 70 degrees) faces: 1. ***Number of non-orthogonality errors: 2131. <<Writing 2132 non-orthogonal faces to set nonOrthoFaces ***Error in face pyramids: 10760 faces are incorrectly oriented. <<Writing 8643 faces with incorrect orientation to set wrongOrientedFaces ***Max skewness = 3.28738e+302, 24 highly skew faces detected which may impair the quality of the results <<Writing 24 skew faces to set skewFaces Coupled point location match (average 0) OK. Failed 8 mesh checks. thanks very much! |
||
December 8, 2015, 06:51 |
|
#4 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
Hi Karelke,
I can't do much with the files from the "sets" folder, because they only provide the lists of indexes and none of them are "-1". Therefore, if the mesh cannot be provided in public, please send me a DropBox link or similar via private message. The output from checkMesh is a considerably great reason for concern, because even hard to believe that solver will not crash with such a mesh. In addition, having the mesh located at such a large distance from the origin of the referential: Code:
(1.12393e+06 -1.69078e+06 -0.5) (1.25165e+06 -1.54424e+06 0.5) Code:
transformPoints -translate '(-1.12393e+06 1.69078e+06 0.0)' -region networkMesh edit: I forgot to ask: What files do you have inside the folder "0/networkMesh"? Best regards, Bruno Last edited by wyldckat; December 8, 2015 at 06:53. Reason: see "edit:" |
|
December 8, 2015, 08:13 |
|
#5 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
Hi Karelke,
I've received the files with success. I'm unable to reproduce the same issue you're getting. I need to know more details, namely:
Bruno |
|
December 8, 2015, 08:32 |
|
#6 | |
Member
Karelke Yu
Join Date: Dec 2014
Posts: 96
Rep Power: 11 |
Quote:
what if you choose the spreadsheet view as shown in the attached image. after that, you can change the Attribute entry from point data to cell data, and sort the sheet by cell type. (see attached image) |
||
December 8, 2015, 09:38 |
|
#7 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
I've tested this just now with OpenFOAM 2.3.0 + ParaView 4.1.0 on Ubuntu 12.04 64-bit, installed from Deb package. What I get is shown in the first (left) attached image.
What fields do you have loaded in the "Volume Sections" on the lower left? In addition, do you have any additional plug-ins loaded? From the menu, choose "Tools -> Manage plugins...". The second (right) image attached shows the default plug-ins that should be loaded. |
|
December 8, 2015, 10:01 |
|
#8 | |
Member
Karelke Yu
Join Date: Dec 2014
Posts: 96
Rep Power: 11 |
Quote:
i think no additional plug-ins are loaded. as attached. and you may need click on the button "Toggle cell connectivity visibility" (shown in the third image) and sort the sheet by cell type. then you can see the pointIndex. |
||
December 8, 2015, 10:26 |
|
#9 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
Quote:
OK, two details:
|
||
December 8, 2015, 22:07 |
|
#10 | |
Member
Karelke Yu
Join Date: Dec 2014
Posts: 96
Rep Power: 11 |
Quote:
Code:
paraFoam -builtin -region networkMesh Code:
paraFoam -region networkMesh -builtin Code:
paraFoam -builtin Code:
ERROR: In /home/yk/OpenFOAM/ThirdParty-2.3.0/ParaView-4.1.0/VTK/IO/Geometry/vtkOpenFOAMReader.cxx, line 6524 vtkOpenFOAMReaderPrivate (0x3a347e0): Wrong list type for uniform field any ideas? best, karelke |
||
December 9, 2015, 17:42 |
|
#11 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,974
Blog Entries: 45
Rep Power: 128 |
Quick answers:
Quote:
Code:
Breakdown of polyhedra by number of faces: faces number of cells 8 29 10 1 In the image is shown up to "Point Index 15", because you have loaded all mesh regions and there should be at least one polyhedral cell that has 16 vertexes (points). |
||
December 9, 2015, 22:10 |
|
#12 |
Member
Karelke Yu
Join Date: Dec 2014
Posts: 96
Rep Power: 11 |
||
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[OpenFOAM.org] Two different versions of ParaView with same OpenFOAM release | FJSJ | OpenFOAM Installation | 2 | July 23, 2017 05:48 |
Paraview version update errors | Dan Pearce | OpenFOAM Installation | 5 | January 8, 2014 05:47 |
Installing OpenFOAM and ParaView in VirtualBox(Ubuntu on Win8) | chrisb2244 | OpenFOAM Installation | 2 | August 21, 2013 13:24 |
Newbie: Install ParaView 3.81 on OF-1.6-ext/OpenSuse 11.2? | lentschi | OpenFOAM Installation | 1 | March 9, 2011 02:32 |
paraFoam reader for OpenFOAM 1.6 | smart | OpenFOAM Installation | 13 | November 16, 2009 21:41 |