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

blockMesh crash with sigFpe

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

Like Tree2Likes
  • 1 Post By wyldckat
  • 1 Post By Mojtaba.a

Reply
 
LinkBack Thread Tools Display Modes
Old   December 6, 2015, 13:24
Question blockMesh crash with sigFpe
  #1
New Member
 
hamide hayati
Join Date: Oct 2015
Posts: 21
Rep Power: 2
hamide is on a distinguished road
hello friends
i wanna block a simple geometry!!! but i face to a problem, it's:

Create time

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3 Foam::Time::readDict() in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#4 Foam::Time::setControls() in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#5 Foam::Time::Time(Foam::word const&, Foam::argList const&, Foam::word const&, Foam::word const&) in "/opt/openfoam220/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#6
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/blockMesh"
#7 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8
in "/opt/openfoam220/platforms/linux64GccDPOpt/bin/blockMesh"
Floating point exception (core dumped)



i don't know what the problem is!!!
would you please help me?
hamide is offline   Reply With Quote

Old   December 6, 2015, 14:01
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,215
Blog Entries: 35
Rep Power: 94
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Quick answer: Not enough information to diagnose the origin of the problem. Please follow the instructions given on this thread: How to give enough info to get help

edit: What you need to do is provide more details about how you got the error in the first place. For example: What is the content of the file "blockMeshDict" that resulted in that crash?

Last edited by wyldckat; December 7, 2015 at 04:56. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Old   December 7, 2015, 06:15
Default
  #3
New Member
 
hamide hayati
Join Date: Oct 2015
Posts: 21
Rep Power: 2
hamide is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Quick answer: Not enough information to diagnose the origin of the problem. Please follow the instructions given on this thread: How to give enough info to get help

edit: What you need to do is provide more details about how you got the error in the first place. For example: What is the content of the file "blockMeshDict" that resulted in that crash?

this is my blockMeshdict:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
    (0 0 0)
    (0.4 0 0)
    (0 0.02 0)
    (0.4 0.02 0)
    (0 0 -0.01)
    (0.4 0 -0.01)
    (0 0.02 -0.01)
    (0.4 0.02 -0.01)
);

blocks
(
    hex (0 1 3 2 4 5 7 6) (100 5 1) simpleGrading (1 1 1)
);

edges
(
);

boundary
(
    inlet
    {
        type patch;
        faces
        (
            (0 2 6 4)
        );
    }
    outlet
    {
         type patch;
         faces
         (
             (1 3 7 5)
         );
     } 
    wall
    {
        type wall;
        faces
        (
            (0 4 5 1)
            (2 6 7 3)
        );
    }
    frontAndBack
    {
        type empty;
        faces
        (
            (0 2 3 1)
            (4 6 7 5)
        );
    }
);

mergePatchPairs
(
);

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

Last edited by wyldckat; December 7, 2015 at 07:24. Reason: Added [CODE][/CODE] markers
hamide is offline   Reply With Quote

Old   December 7, 2015, 07:35
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,215
Blog Entries: 35
Rep Power: 94
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Hamide,

I've gotten a very different result from the one you reported:
Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.0-5be49240882f
Exec   : blockMesh
Date   : Dec 07 2015
Time   : 11:25:55
Host   : "machine"
PID    : 14207
Case   : /home/ofuser/OpenFOAM/ofuser-2.2.0/run/hamide/cavity
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Creating block mesh from
    "/home/ofuser/OpenFOAM/ofuser-2.2.0/run/hamide/cavity/constant/polyMesh/blockMeshDict"
Creating curved edges
Creating topology blocks
Creating topology patches

Creating block mesh topology
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.33333e-05 for face 0
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.33333e-05 for face 1
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.33333e-05 for face 2
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.33333e-05 for face 3
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.33333e-05 for face 4
--> FOAM Warning : 
    From function cellModel::mag(const labelList&, const pointField&)
    in file meshes/meshShapes/cellModel/cellModel.C at line 128
    zero or negative pyramid volume: -1.33333e-05 for face 5
--> FOAM Warning : 
    From function blockMesh::createTopology(IOdictionary&)
    in file blockMesh/blockMeshTopology.C at line 255
    negative volume block : 0, probably defined inside-out

Check topology

  Basic statistics
    Number of internal faces : 0
    Number of boundary faces : 6
    Number of defined boundary faces : 6
    Number of undefined boundary faces : 0
  Checking patch -> block consistency

Creating block offsets
Creating merge list .

Creating polyMesh from blockMesh
Creating patches
Creating cells
Creating points with scale 1

Writing polyMesh
----------------
Mesh Information
----------------
  boundingBox: (0 0 -0.01) (0.4 0.02 0)
  nPoints: 1212
  nCells: 500
  nFaces: 2105
  nInternalFaces: 895
----------------
Patches
----------------
  patch 0 (start: 895 size: 5) name: inlet
  patch 1 (start: 900 size: 5) name: outlet
  patch 2 (start: 905 size: 200) name: wall
  patch 3 (start: 1105 size: 1000) name: frontAndBack

End
The problem is that the order of the vertices is incorrect. Please study the OpenFOAM User Guide in more detail. You can find the location of the PDF file if you run this command:
Code:
echo $WM_PROJECT_DIR/doc/Guides-a4/UserGuide.pdf
The other possibility is for you to install OpenFOAM 3.0.0, because that version allows for any order of the vertices.

Best regards,
Bruno
__________________
___
I'll be at OFW11 in Portugal
wyldckat is offline   Reply With Quote

Old   December 7, 2015, 09:48
Default
  #5
New Member
 
hamide hayati
Join Date: Oct 2015
Posts: 21
Rep Power: 2
hamide is on a distinguished road
thank you very much
but i cant understand what you mean!!!!
do you mean i should make the finer mesh?
i don't know how improve it!!!!!!
hamide is offline   Reply With Quote

Old   December 7, 2015, 09:55
Default
  #6
New Member
 
hamide hayati
Join Date: Oct 2015
Posts: 21
Rep Power: 2
hamide is on a distinguished road
and the other problem is:
i'm new in openFoam. i just can run it's tutorial and change them according to my need...
i can block this geometry in pisoFoam algorithm tutorial but not in the simpleFoam!!!!!
the error i sent you was in simpleFoam algorithm tutorial
hamide is offline   Reply With Quote

Old   December 7, 2015, 13:38
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,215
Blog Entries: 35
Rep Power: 94
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Hamide,

Quote:
Originally Posted by hamide View Post
but i cant understand what you mean!!!!
do you mean i should make the finer mesh?
I mean that the problem is explained in section 5.3 in the User Guide: http://cfd.direct/openfoam/user-guide/blockMesh/

The problem you have is with the way the vertices are ordered:
Code:
vertices
(
    (0 0 0)
    (0.4 0 0)
    (0 0.02 0)
    (0.4 0.02 0)
    (0 0 -0.01)
    (0.4 0 -0.01)
    (0 0.02 -0.01)
    (0.4 0.02 -0.01)
);
And also the way they are ordered in the "faces" lists. For example, one of the problems could be this:
Code:
        faces
        (
            (0 2 6 4)
        );
The problem might be that the correct order is possibly "(4 2 6 0)", but I don't know if that is the solution or not.

Quote:
Originally Posted by hamide View Post
i'm new in openFoam. i just can run it's tutorial and change them according to my need...
i can block this geometry in pisoFoam algorithm tutorial but not in the simpleFoam!!!!!
the error i sent you was in simpleFoam algorithm tutorial
Have you studied the 3 tutorials from the User Guide? See here: http://cfd.direct/openfoam/user-guide/tutorials/

Then you should take one step at a time. One small change and then test. Practice with each tutorial case. Learn how each detail works. Only then you should try and change to another tutorial.

Best regards,
Bruno
hamide likes this.
wyldckat is offline   Reply With Quote

Old   December 13, 2015, 14:51
Default
  #8
Senior Member
 
Mojtaba.a's Avatar
 
Mojtaba Amiraslanpour
Join Date: Jun 2011
Location: Zanjan, Iran
Posts: 263
Rep Power: 7
Mojtaba.a is on a distinguished road
Send a message via Yahoo to Mojtaba.a
Quote:
Originally Posted by hamide View Post
and the other problem is:
i'm new in openFoam. i just can run it's tutorial and change them according to my need...
i can block this geometry in pisoFoam algorithm tutorial but not in the simpleFoam!!!!!
the error i sent you was in simpleFoam algorithm tutorial
Hi,

As wyldcat said you have to be careful with vertices order. I have completely taught the basics of blockMesh using the famous cavity problem OF in here.
If you had any other questions, you may ask here to get more detailed answers.

Soon there will be a Persian book out regarding "Meshing in OpenFOAM".

Best.
hamide likes this.
__________________
Learn OpenFOAM in Persian for free, And ask your questions here.
Complex Heat & Flow Simulation Research Group
If you can't explain it simply, you don't understand it well enough. "Richard Feynman"
Mojtaba.a is online now   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
Is Playstation 3 cluster suitable for CFD work hsieh OpenFOAM 9 August 16, 2015 14:53
External flow around cube with blockMesh Woody8 OpenFOAM Native Meshers: blockMesh 0 March 31, 2015 14:54
set of xyz data in blockMesh psk OpenFOAM Native Meshers: blockMesh 12 August 27, 2013 08:37
tutorial 2.2 Stress(...) trouble with blockMesh colinB OpenFOAM Native Meshers: blockMesh 8 January 22, 2012 11:32
Blockmesh cavity error message tonitoney OpenFOAM Installation 2 March 17, 2008 12:59


All times are GMT -4. The time now is 08:27.