CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Native Meshers: blockMesh

Plot3dToFoam mesh conversion error

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 21, 2006, 13:34
Default While trying to convert a plot
  #1
New Member
 
Ram Poudel
Join Date: Mar 2009
Location: Flagstaff, arizona, USA
Posts: 9
Rep Power: 8
rcpoudel is on a distinguished road
While trying to convert a plot3d volume mesh generated in Overgrid using Hypgen, I encounter the following error:
---------------------------------------------------
Exec : plot3dToFoam .. cavity /home/rcpoudel/aubrey/av80fsn.p3d
Date : Dec 21 2006
Time : 10:32:25
Host : venus
PID : 10975
Root : ..
Case : cavity
Nprocs : 1
Create time

Reading 93 blocks


--> FOAM FATAL IO ERROR : wrong token type - expected int found on line 2 the doubleScalar 368860

file: /home/rcpoudel/aubrey/av80fsn.p3d at line 2.

From function operator>>(Istream&, int&)
in file primitives/int/intIO.C at line 74.

FOAM exiting
---------------------------------------------------

Few lines of the p3d volume grid file I want to convert to Foam format are as follows:
93 133 51
0.3688602E+06 0.3690820E+06 0.3693038E+06 0.3695257E+06 0.3697475E+06
0.3699694E+06 0.3701912E+06 0.3704131E+06 0.3706349E+06 0.3708568E+06
0.3710786E+06 0.3713004E+06 0.3715223E+06 0.3717441E+06 0.3719660E+06
0.3721878E+06 0.3724097E+06 0.3726315E+06 0.3728533E+06 0.3730752E+06
0.3732970E+06 0.3735189E+06 0.3737407E+06 0.3739626E+06 0.3741844E+06
0.3744063E+06 0.3746281E+06 0.3748499E+06 0.3750718E+06 0.3752936E+06
0.3755154E+06 0.3757373E+06 0.3759591E+06 0.3761810E+06 0.3764028E+06
0.3766247E+06 0.3768465E+06 0.3770684E+06 0.3772902E+06 0.3775120E+06
0.3777339E+06 0.3779557E+06 0.3781776E+06 0.3783994E+06 0.3786213E+06
--------------------------------------------------

Any help to fix this error will be highly appreciated.

Thanks in advance,

Ram
rcpoudel is offline   Reply With Quote

Old   December 21, 2006, 18:43
Default from the Description field of
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
from the Description field of the source plot3dToFoam.C):
- multi block ascii by default
- expects blanking

Does your mesh have 93 blocks? Your first line looks more like a Ni x Nj x Nk block dimension.

What happens if you run plot3dToFoam in single-block mode?
mattijs is offline   Reply With Quote

Old   December 22, 2006, 14:42
Default Mattijs, The volume grid is
  #3
New Member
 
Ram Poudel
Join Date: Mar 2009
Location: Flagstaff, arizona, USA
Posts: 9
Rep Power: 8
rcpoudel is on a distinguished road
Mattijs,

The volume grid is a single block with no iblanks.
Yes the first line is xDim:93 yDim:133 zDim:51

When I try to execute:
[rcpoudel@venus turbFoam]$ plot3dToFoam -singleBlock -noBlank . cavity ~/aubrey/av80fsn.p3d > log & cat log
[1] 26719

The log file displays thousands of lines like:
(1) Cannot determine orientation of cell 35 128 0 since has base vectors (221.8 0 41.371)(0 275 -12.065)(0 0 0)

(2) Checking mesh
--> FOAM Warning :
From function bool primitiveMesh::checkPoints(const bool, labelHashSet*) const
in file meshes/primitiveMesh/primitiveMeshCheck.C at line 884
Point 7613 not used by any faces.

3) And the following lines appear on the display:

Foam::error::printStack(Foam:stream&)
Foam::sigSegv::sigSegvHandler(int)
/lib64/tls/libc.so.6 [0x35b9a2e410]
Foam::cell::labels(Foam::UList<foam::face> const&) const
Foam::primitiveMesh::calcPointCells() const
Foam::primitiveMesh::pointCells() const
Foam::primitiveMesh::checkPoints(bool, Foam::HashSet<int,> >*) const
Foam::primitiveMesh::checkTopology(bool) const
Foam::primitiveMesh::checkMesh(bool) const
plot3dToFoam [0x406a50]
__libc_start_main
__gxx_personality_v0
---------------------------------------------------

Regards,
Ram
rcpoudel is offline   Reply With Quote

Old   December 25, 2006, 12:32
Default All, I convert a plot3d Mes
  #4
New Member
 
Ram Poudel
Join Date: Mar 2009
Location: Flagstaff, arizona, USA
Posts: 9
Rep Power: 8
rcpoudel is on a distinguished road
All,

I convert a plot3d Mesh to Foam. Viewing it on paraFoam looks okey.

How can I identify the nFaces and startFace number as required by boundary file of /constant/polyMesh directory to specify inlet, outlet and wall and slip wall etc. My "boundary" file contain only one face for wall as follows:
(
defaultFaces
{
type wall;
nFaces 46688;
startFace 1798256;
}
)


My domain is somewhat cuboid.

------------------------------------
velocity-inlet
{
type patch;
nFaces ????;
startFace ?????;
}

pressure-outlet
{
type patch;
nFaces ????;
startFace ????;
}
)
--------------------------------------
How to identify the numbers "?????"..

Is there any mesh manipulation utility (e.g. autoPatch) that can do this job for me?

Thanks,

Ram Poudel
rcpoudel is offline   Reply With Quote

Old   December 25, 2006, 12:34
Default All, I convert a plot3d Mes
  #5
New Member
 
Ram Poudel
Join Date: Mar 2009
Location: Flagstaff, arizona, USA
Posts: 9
Rep Power: 8
rcpoudel is on a distinguished road
All,

I convert a plot3d Mesh to Foam. Viewing it on paraFoam looks okey.

How can I identify the nFaces and startFace number as required by boundary file of /constant/polyMesh directory to specify inlet, outlet and wall and slip wall etc. My "boundary" file contain only one face for wall as follows:
(
defaultFaces
{
type wall;
nFaces 46688;
startFace 1798256;
}
)


My domain is somewhat cuboid.

------------------------------------
velocity-inlet
{
type patch;
nFaces ????;
startFace ?????;
}

pressure-outlet
{
type patch;
nFaces ????;
startFace ????;
}
)
--------------------------------------
How to identify the numbers "?????"..

Is there any mesh manipulation utility (e.g. autoPatch) that can do this job for me?

Thanks,

Ram Poudel
rcpoudel is offline   Reply With Quote

Old   January 1, 2007, 09:19
Default - autoPatch if you have sharp
  #6
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
- autoPatch if you have sharp features (e.g. for cube it will create 6 patches)
- use faceSet to collect faces you want to make into a patch and run createPatch.
mattijs is offline   Reply With Quote

Old   April 1, 2008, 06:50
Default Hi everybody, I'm trying to
  #7
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
Hi everybody,

I'm trying to import a 2d naca profile written in Plot3d but I get the following error:

Exec : plot3dToFoam /home/dino/OpenFOAM/dino-1.4.1/run/tutorials/potentialFoam/ nacaPotential naca_0012.xyz
Date : Mar 29 2008
Time : 11:51:46
Host : ime054
PID : 5316
Root : /home/dino/OpenFOAM/dino-1.4.1/run/tutorials/potentialFoam/
Case : nacaPotential
Nprocs : 1
Create time

Reading 1 blocks
xDim:257 yDim:129 zDim:1
Reading block points
block 0:


--> FOAM FATAL IO ERROR : Attempt to get back from bad stream

file: naca_0012.xyz at line 5.

From function void Istream::getBack(token& t)
in file db/IOstreams/IOstreams/Istream.C at line 44.

FOAM exiting

I don't know if this utilities needs a 3d mesh to convert, but if I remember correctly openfoam automatically introduce a third dimension. Moreover I've tried with a 3d mesh as well and I get the same message.
Thank you in advance for any support.

dino
dinonettis is offline   Reply With Quote

Old   April 1, 2008, 14:39
Default Is it a single block case? Any
  #8
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Is it a single block case? Any of the options help? -noBlank, -singleBlock.
mattijs is offline   Reply With Quote

Old   April 2, 2008, 03:47
Default yes it is a single block case.
  #9
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
yes it is a single block case. anyway if it can help you this is the initial part of the file:


1
257 129 2
51.0000000000000 42.1102600097656 34.8004417419434 28.7897491455078 23.8472995758057 19.7832393646240 16.4414691925049 13.6935997009277 11.4341001510620 9.57616806030273 8.04843330383301 6.79221296310425 5.75925302505493 4.90987491607666 4.21145200729370 3.63715505599976 3.16492509841919 2.77662110328674 2.45732808113098 2.19478106498718 1.97889494895935 1.80137705802917 1.65540897846222 1.53538203239441 1.43668699264526 1.35553205013275 1.28880095481873 1.23392903804779 1.18880999088287 1.15170896053314 1.12120199203491 1.09611594676971 1.07548904418945 1.05852794647217 1.04458200931549 1.03311395645142 1.02368402481079 1.01593005657196 1.00955402851105 1.00431096553802 1.00000000000000 0.995899498462677 0.991405487060547 0.986484289169312 0.981100320816040



thank you in advance

dino
dinonettis is offline   Reply With Quote

Old   April 2, 2008, 04:29
Default Can you attach the file here o
  #10
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Can you attach the file here or send it to me? m dot janssens at the opencfd.co.uk domain.
mattijs is offline   Reply With Quote

Old   April 3, 2008, 14:21
Default Attached a version of plot3DTo
  #11
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Attached a version of plot3DToFoam which handles 2D files. Specify a thickness with the -2D option.

plot3dToFoam root case file -noBlank -2D 1

plot3dToFoam.tgz
mattijs is offline   Reply With Quote

Old   April 4, 2008, 07:41
Default Hi Mattijs, the new version
  #12
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
Hi Mattijs,
the new version works good with 2d mesh, but when I run the checkmesh this is the message that I get. Do you think that this issue, concerning high aspect ratio cells, can be ignored??
Thanks

dino


Exec : checkMesh /home/nettis/OpenFOAM/nettis-1.4.1/run/tutorials/potentialFoam nacaPotential
Date : Apr 04 2008
Time : 13:29:40
Host : ime171
PID : 11008
Root : /home/nettis/OpenFOAM/nettis-1.4.1/run/tutorials/potentialFoam
Case : nacaPotential
Nprocs : 1
Create time

Create polyMesh for time = constant

Time = constant

Mesh stats
points: 66224
edges: 164872
faces: 131416
internal faces: 65192
cells: 32768
boundary patches: 1
point zones: 0
face zones: 0
cell zones: 0

Number of cells of each type:
hexahedra: 32768
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Topological cell zip-up check OK.
Face vertices OK.
Face-face connectivity OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface
defaultFaces 66224 66224 ok (closed singly connected surface)

Checking geometry...
Domain bounding box: (-48.2397 -51.0969 0) (51 51.0969 1)
Boundary openness (1.96518e-18 -7.86073e-19 0) OK.
***High aspect ratio cells found, Max aspect ratio: 7.07665e+06, number of cells 14028
<<Writing 14028 cells with high aspect ratio to set highAspectRatioCells
Minumum face area = 5.44474e-10. Maximum face area = 49.7139. Face area magnitudes OK.
Min volume = 5.44474e-10. Max volume = 49.7139. Total volume = 8860.64. Cell volumes OK.
Mesh non-orthogonality Max: 87.6327 average: 8.50995
*Number of severely non-orthogonal faces: 422.
Non-orthogonality check OK.
<<Writing 422 non-orthogonal faces to set nonOrthoFaces
Face pyramids OK.
Max skewness = 0.188965 OK.
*Edges too small, min/max edge length = 1.24797e-06 8.88974, number too small: 19422
<<Writing 19854 points on short edges to set shortEdges
All angles in faces OK.
Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1
All face flatness OK.

Failed 1 mesh checks.

End

Actually I can use the empty bc in the third direction, is it correct?
dinonettis is offline   Reply With Quote

Old   April 4, 2008, 09:13
Default ps: since this is the first ti
  #13
Member
 
Leonardo Nettis
Join Date: Mar 2009
Posts: 72
Rep Power: 8
dinonettis is on a distinguished road
ps: since this is the first time I work with plot3d format (up to now I created .msh files with gambit) I don't know how to impose certain boundary conditions on specific patches. In fact once I import the mesh with plot3dto Foam, all the faces are added to a default patch whilst when I work with gambit I can specify the boundary type in gambit and then thay are imported in OF. Could you give me some advices??
This is the warning message I get:

Creating boundary patches
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 577
Found 66224 undefined faces in mesh; adding to default patch.

Thank you in advance.

dino
dinonettis is offline   Reply With Quote

Old   November 4, 2008, 16:48
Default I had the same problem when I
  #14
New Member
 
Peter Lian
Join Date: Mar 2009
Posts: 12
Rep Power: 8
peter73 is on a distinguished road
I had the same problem when I converted the plot3d file to the openfoam file. Does anyone have a solution?

Mattijs suggested autoPatch. But I still cannot get the right files.


Peter
peter73 is offline   Reply With Quote

Old   November 10, 2008, 13:42
Default Hi, I have the same issues. M
  #15
New Member
 
Shawn Westmoreland
Join Date: Mar 2009
Location: Huntsville, AL, USA
Posts: 1
Rep Power: 0
wshawnw is on a distinguished road
Hi, I have the same issues. Many plot3d grids that I would like to use but not sure how to go about setting the boundary conditions after running plot3dToFoam. Is there any way in paraFoam to see the face/node indexing?
Thanks,
Shawn
wshawnw is offline   Reply With Quote

Old   July 11, 2010, 17:18
Default Plot3Dtofoam
  #16
New Member
 
Join Date: Jul 2010
Posts: 17
Rep Power: 6
hm86 is on a distinguished road
Hey all,
I am trying to convert a plot3d mesh file for use in openFOAM. I get the following when I use

plot3dtofoam mesh.p3d -noBlank

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.7.0-279cc8e8233b
Exec : plot3dToFoam mesh.p3d -noBlank
Date : Jul 11 2010
Time : 09:30:49
Host : remote-desktop
PID : 3755
Case : /home/remote/OpenFOAM/remote-1.7.0/run/test/test
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Reading 5 blocks
block 0 nx:201 ny:211 nz:1
block 1 nx:201 ny:211 nz:1
block 2 nx:201 ny:211 nz:1
block 3 nx:201 ny:211 nz:1
block 4 nx:100 ny:100 nz:1
Reading block points
block 0:
Reading 42411 x coordinates...
Reading 42411 y coordinates...
Reading 42411 z coordinates...
--> FOAM Warning :
From function hexBlock::hexBlock::setHandedness()
in file hexBlock.C at line 89
Cannot determine orientation of block. Continuing as if right handed.

block 1:
Reading 42411 x coordinates...
Reading 42411 y coordinates...
Reading 42411 z coordinates...
--> FOAM Warning :
From function hexBlock::hexBlock::setHandedness()
in file hexBlock.C at line 89
Cannot determine orientation of block. Continuing as if right handed.

block 2:
Reading 42411 x coordinates...
Reading 42411 y coordinates...
Reading 42411 z coordinates...
--> FOAM Warning :
From function hexBlock::hexBlock::setHandedness()
in file hexBlock.C at line 89
Cannot determine orientation of block. Continuing as if right handed.

block 3:
Reading 42411 x coordinates...
Reading 42411 y coordinates...
Reading 42411 z coordinates...
--> FOAM Warning :
From function hexBlock::hexBlock::setHandedness()
in file hexBlock.C at line 89
Cannot determine orientation of block. Continuing as if right handed.

block 4:
Reading 10000 x coordinates...
Reading 10000 y coordinates...
Reading 10000 z coordinates...
--> FOAM Warning :
From function hexBlock::hexBlock::setHandedness()
in file hexBlock.C at line 89
Cannot determine orientation of block. Continuing as if right handed.

Merged points within 1e-15 distance. Merged from 179644 down to 177672 points.
Creating cells
Creating boundary patches
Writing polyMesh
End

When I open the owner file in constant/polyMesh, i get

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.7.0 |
| \\ / A nd | Web: www.OpenFOAM.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class labelList;
note "nPoints: 177672 nCells: 0 nFaces: 0 nInternalFaces: 0";
location "constant/polyMesh";
object owner;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

0()

// ************************************************** *********************** //

I dont know why there are no cells or faces. Anyone encounter similar problems or have any ideas on why this might be happening? or any solutions?

Thanks!
hm86 is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Star mesh conversion Mattijs Janssens (Mattijs) OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 34 November 14, 2008 06:00
Plot3DtoFoam conversion error dinonettis OpenFOAM Meshing Format & General Technical 0 March 29, 2008 07:03
polyhedral mesh conversion ali FLUENT 4 September 14, 2007 11:55
About mesh conversion Spyros CD-adapco 0 January 5, 2007 21:18
Error while running plot3dToFoam ploceus OpenFOAM Pre-Processing 1 December 14, 2005 05:55


All times are GMT -4. The time now is 01:23.