CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   channelFoam for a 3D pipe (http://www.cfd-online.com/Forums/openfoam/82849-channelfoam-3d-pipe.html)

AlmostSurelyRob December 7, 2010 14:01

channelFoam for a 3D pipe
 
1 Attachment(s)
Dear All,

I would value your advice on the case I am trying to set up. Basically I wish to adapt channelFoam tutorial to a certain type of 3D pipeline mesh. (see attached).

I believe I have already sorted out the meshing. However blockMesh still gives me an output with warnings about negative volumes.

Code:

/*---------------------------------------------------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.7.1                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.com                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
Build  : 1.7.1-03e7e056c215
Exec  : blockMesh
Date  : Dec 07 2010
Time  : 17:44:19
Host  : soli31888c
PID    : 28450
Case  : /home/c111269/OpenFOAM/c111269-1.7.1/cases
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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


Creating block mesh from
    "/home/c111269/OpenFOAM/c111269-1.7.1/cases/constant/polyMesh/blockMeshDict"


Creating blockCorners

Creating curved edges

Creating blocks

Creating 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: -0.666667 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: -0.666667 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: -0.666667 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: -0.666667 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: -0.666667 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: -0.666667 for face 5
--> FOAM Warning :
    From function blockMesh::createTopology(IOdictionary&)
    in file createTopology.C at line 397
    negative volume block : 0, probably defined inside-out
--> 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: -0.5 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: -0.5 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: -0.5 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: -0.5 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: -0.333333 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: -0.666667 for face 5
--> FOAM Warning :
    From function blockMesh::createTopology(IOdictionary&)
    in file createTopology.C at line 397
    negative volume block : 1, probably defined inside-out
--> 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: -0.5 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: -0.5 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: -0.5 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: -0.5 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: -0.333333 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: -0.666667 for face 5
--> FOAM Warning :
    From function blockMesh::createTopology(IOdictionary&)
    in file createTopology.C at line 397
    negative volume block : 2, probably defined inside-out
--> 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: -0.5 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: -0.5 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: -0.5 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: -0.5 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: -0.333333 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: -0.666667 for face 5
--> FOAM Warning :
    From function blockMesh::createTopology(IOdictionary&)
    in file createTopology.C at line 397
    negative volume block : 3, probably defined inside-out
--> 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: -0.5 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: -0.5 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: -0.5 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: -0.5 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: -0.333333 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: -0.666667 for face 5
--> FOAM Warning :
    From function blockMesh::createTopology(IOdictionary&)
    in file createTopology.C at line 397
    negative volume block : 4, probably defined inside-out

Default patch type set to empty

Check block mesh topology

        Basic statistics
                Number of internal faces : 8
                Number of boundary faces : 14
                Number of defined boundary faces : 14
                Number of undefined boundary faces : 0

        Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points with scale 1

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Writing polyMesh

End

I construct this mesh by creating the cube in the centre, adding the surrounding edges and than creating blocks for each section. Please, note that the number of outer and internal faces is correct.

Here's my blockMeshDict:
Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.7.1                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.com                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices       
(
//internal square
    (0 -1 -1) //0
    (1 -1 -1) //1
    (1 -1  1) //2
    (0 -1  1) //3
    (0  1 -1) //4
    (1  1 -1) //5
    (1  1  1) //6
    (0  1  1) //7
//Going clockwise with sections
//North section
    (0  2  2) //8
    (0 -2  2) //9
    (1  2  2) //10
    (1 -2  2) //11
//East section
    (0  2 -2) //12
    (1  2 -2) //13
//South section
    (0 -2 -2) //14
    (1 -2 -2) //15
);

edges         
(
//North section
  arc  8  9 (0  0    2.82)
  arc 10 11 (1  0    2.82)
//East section
  arc  8 12 (0  2.82  0)
  arc 10 13 (1  2.82  0)
//South section
  arc 12 14 (0  0 -2.82 )
  arc 13 15 (1  0 -2.82 )
//West section
  arc 14  9 (0  -2.82 0)
  arc 15 11 (1  -2.82 0)
);

blocks         
(
//Centre
    hex (0 1 2 3 4 5 6 7) (32 48 48) simpleGrading (1 1 1)
//East section
    hex (7 6 2 3 8 10 11 9) (32 48 92) simpleGrading (1 1 0.25)
//East section
    hex (4 5 6 7 12 13 10 8) (32 48 92) simpleGrading (1 1 0.25)
//South section
    hex (0 1 5 4 14 15 13 12) (32 48 92) simpleGrading (1 1 0.25)
//West section
    hex (3 2 1 0 9 11 15 14) (32 48 92) simpleGrading (1 1 0.25)
);

patches       
(
    wall pipeWall
    (
        (9 11 10 8)
        (8 10 13 12)
        (12 14 15 13)
        (14 9 11 15)
    )
    cyclic cNorth
    (
        (9  3 7  8)
        (11 2 6 10)
    )
    cyclic cEast
    (
        (7  4 12  8)
        (6  5 13 10)
    )
    cyclic cSouth
    (
        (0 14 12 4)
        (1 5 13 15)
    )
    cyclic cWest
    (
        (0 14 9 3)
        (1 15 11 2)
    )
    cyclic cCentre
    (
        (0 4 7 3)
        (1 2 6 5)
    )
);

mergePatchPairs
(
);

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


After setting up all other dictionaries, running channelFoam results in an error:

Code:

/*---------------------------------------------------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.7.1                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.com                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
Build  : 1.7.1-03e7e056c215
Exec  : channelFoam
Date  : Dec 07 2010
Time  : 17:46:09
Host  : soli31888c
PID    : 28478
Case  : /home/c111269/OpenFOAM/c111269-1.7.1/cases
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0

                                                                                                                                                                                   
Reading transportProperties                                                                                                                                                       
                                                                                                                                                                                   
Reading field p                                                                                                                                                                   
                                                                                                                                                                                   
Reading field U                                                                                                                                                                   
                                                                                                                                                                                   
Reading/calculating face flux field phi                                                                                                                                           
                                                                                                                                                                                   
Selecting incompressible transport model Newtonian                                                                                                                                 
Selecting LES turbulence model oneEqEddy                                                                                                                                           
oneEqEddyCoeffs                                                                                                                                                                   
{                                                                                                                                                                                 
    ce              1.048;                                                                                                                                                         
    ck              0.094;                                                                                                                                                         
}                                                                                                                                                                                 
                                                                                                                                                                                   
Initializing with 0 pressure gradient                                                                                                                                             
                                                                                                                                                                                   
                                                                                                                                                                                   
Starting time loop
                                                                                                                                                                                   
Reading/calculating field UMean                                                                                                                                                   
                                                                                                                                                                                   
Reading/calculating field pMean                                                                                                                                                   
                                                                                                                                                                                   
Reading/calculating field UPrime2Mean                                                                                                                                             

Reading/calculating field pPrime2Mean

fieldAverage: starting averaging at time 0

Time = 0.02

Courant Number mean: 0.519785 max: 1.7088
#0  Foam::error::printStack(Foam::Ostream&) in "/home/c111269/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#1  Foam::sigFpe::sigFpeHandler(int) in "/home/c111269/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libOpenFOAM.so"
#2  in "/lib64/libc.so.6"
#3  void Foam::magSqr<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh> const&) in "/home/c111269/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#4  Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::magSqr<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<Foam::SymmTensor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/c111269/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#5  Foam::incompressible::LESModels::oneEqEddy::correct(Foam::tmp<Foam::GeometricField<Foam::Tensor<double>, Foam::fvPatchField, Foam::volMesh> > const&) in "/home/c111269/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#6  Foam::incompressible::LESModel::correct() in "/home/c111269/OpenFOAM/OpenFOAM-1.7.1/lib/linux64GccDPOpt/libincompressibleLESModels.so"
#7 
 in "/home/c111269/OpenFOAM/OpenFOAM-1.7.1/applications/bin/linux64GccDPOpt/channelFoam"
#8  __libc_start_main in "/lib64/libc.so.6"
#9 
 at /usr/src/packages/BUILD/glibc-2.11.2/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception

which I guess means that it's diverging.

My questions are

1) Can I run channelFoam for any other geometry than channel?
2) Why do I get warnings about negative volumes?
3) Do I have to specify each cyclic patch separately?

Please let me know if you know of any other references on running 3D pipeline simulation in openFoam with cyclic boundary conditions. It would be great if you could advise me if I am on the right track at least with setting up my case.

Many thanks,
Robert

MartinB December 7, 2010 14:19

Hi Robert,

change your block definition to:
Code:

blocks         
(
//Centre
    hex (4 5 6 7 0 1 2 3) (32 48 48) simpleGrading (1 1 1)
//East section
    hex (8 10 11 9 7 6 2 3) (32 48 92) simpleGrading (1 1 0.25)
//East section
    hex (12 13 10 8 4 5 6 7) (32 48 92) simpleGrading (1 1 0.25)
//South section
    hex (14 15 13 12 0 1 5 4) (32 48 92) simpleGrading (1 1 0.25)
//West section
    hex (9 11 15 14 3 2 1 0) (32 48 92) simpleGrading (1 1 0.25)
);

Then the negative volumes are gone. Don't know about the rest, but may be it's running now...

Martin

AlmostSurelyRob December 7, 2010 14:41

Thanks Martin for such prompt and accurate reply. Yes the negative volumes were the issue. Now the simulation runs smoothly. I an eagerly waiting for some results now.

I am awfully sorry! Have I violated the right-hand side rule?

albem June 24, 2011 13:06

Hello

Could anybody help me to fix a grid for a square channel with curved edges?

Any reference is welcome

thanks in advance

Alberto


All times are GMT -4. The time now is 13:13.