[bshambaugh]

I am having trouble with a boundary that involves a changing grid density. I think I need to use cyclicAMI instead of cyclic. There was a post with this question in 2012 about this linked to below.


The mesh looks like this:




Observe that there are 20 faces on the left and 40 faces on the right of the boundary in the center.


The error message is:

For patch leftRightWallleft there are 20 face centres, for the neighbour patch leftRightWallsright there are 40                        
                          From function void Foam::cyclicPolyPatch::calcTransforms(const primitivePatch&, const pointField&, const vectorField&, const pointField&, const vectorField&)                           in file meshes/polyMesh/polyPatches/constraint/cyclic/cyclicPolyPatch.C at line 156.--> FOAM FATAL ERROR:

Is getting cyclicAMI to work as easy as replacing cyclic with cyclicAMI? Doing this replacement does not seem to work.

e.g.

leftRightWallleft  
    {
        type            cyclic;
        neighbourPatch    leftRightWallsright;
        nFaces          20;
        startFace       4720;
}

to

leftRightWallleft  
    {
        type            cyclicAMI;
        neighbourPatch    leftRightWallsright;
        nFaces          20;
        startFace       4720;
}

I am borrowing from the 2012 version of this question, cyclic boundary with same geometric size but different number of faces?

For my Files, I replaced cyclic with cyclicAMI. (https://github.com/bshambaugh/openfo...lbow-twoFaces/)

in constant/polyMesh/boundary

leftRightWallleft  
    {
        type            cyclicAMI;   
        neighbourPatch    leftRightWallsright;
        nFaces          20;
        startFace       4720;
}

 leftRightWallsright
    {
        type            cyclicAMI;
        neighbourPatch  leftRightWallleft;
        nFaces          40;
        startFace       4760;
}

in 0/p

leftRightWallleft
    {
        type            cyclicAMI;
        nFaces          20;
        startFace       4720;
}

    leftRightWallsright
    {
        type            cyclicAMI;
        nFaces          40;
        startFace       4760;
}

in 0/U

leftRightWallleft
    {
        type            cyclicAMI;
        nFaces          20;
        startFace       4720;
}

    leftRightWallsright
    {
        type            cyclicAMI;
        nFaces          40;
        startFace       4760;
}

[bshambaugh]

This is a compound mesh that was created in Salome, and then modified to work with OpenFoam. A method similar to what I used is described here [1].


To solve this problem, I will look at Glue Faces in Salome [2], and MergeMesh and StitchMesh in OpenFoam [3].

Edit: Bookmarking this. It seems close. Problem using AMI

[1] http://staff.um.edu.mt/__data/assets...o_OpenFOAM.pdf
[2] http://www.salome-platform.org/forum/forum_10/818415930
[3] MergeMesh and stitchMesh

[bshambaugh]

I ran the code and I obtained in log.icoFoam: "
"ill defined primitiveEntry starting at keyword 'value' ..."

Below is log.icoFoam followed by the constant/polyMesh/boundary,
0/p and 0/U configuration files.

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 4.1
Exec   : icoFoam
Date   : Nov 10 2018
Time   : 15:33:30
Host   : "caelinux"
PID    : 30779
Case   : /home/caelinux/OpenFOAM/caelinux-4.1/run/tutorials/incompressible/icoFoam/elbow-fchannel
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0


PISO: Operating solver in PISO mode

Reading transportProperties

Reading field p

AMI: Creating addressing and weights between 40 source faces and 20 target faces
AMI: Patch source sum(weights) min/max/average = 1, 1, 1
AMI: Patch target sum(weights) min/max/average = 1, 1, 1
Reading field U



--> FOAM FATAL IO ERROR: 
"ill defined primitiveEntry starting at keyword 'value' on line 63 and ending at line 69"

file: /home/caelinux/OpenFOAM/caelinux-4.1/run/tutorials/incompressible/icoFoam/elbow-fchannel/0/U at line 69.

    From function void Foam::primitiveEntry::readEntry(const Foam::dictionary&, Foam::Istream&)
    in file db/dictionary/primitiveEntry/primitiveEntryIO.C at line 189.

FOAM exiting

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

10
(
    leftRightWallsright
    {
        type            cyclicAMI;
        neighbourPatch  leftRightWallleft;
        transform       noOrdering;
        nFaces          40;
        startFace       3880;
    }
    outlet
    {
        type            patch;
        nFaces          40;
        startFace       3920;
    }
    channelWallsright
    {
        type            wall;
        nFaces          80;
        startFace       3960;
    }
    destinationFaceright
    {
        type            wall;
        nFaces          1600;
        startFace       4040;
    }
    sourceFaceright
    {
        type            wall;
        nFaces          1600;
        startFace       5640;
    }
    sourceFaceleft
    {
        type            wall;
        nFaces          400;
        startFace       7240;
    }
    destinationFaceleft
    {
        type            wall;
        nFaces          400;
        startFace       7640;
    }
    channelWallsleft
    {
        type            wall;
        nFaces          40;
        startFace       8040;
    }
    leftRightWallleft
    {
        type            cyclicAMI;
        neighbourPatch  leftRightWallsright;
        transform       noOrdering;
        nFaces          20;
        startFace       8080;
    }
    inlet
    {
        type            patch;
        nFaces          20;
        startFace       8100;
    }
)

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

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    leftRightWallsright
    {
        type            cyclicAMI;
    }
    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }
    channelWallsright
    {
        type            zeroGradient;
    }
    destinationFaceright
    {
        type            zeroGradient;
    }
    sourceFaceright
    {
        type            zeroGradient;
    }
    sourceFaceleft
    {
        type            zeroGradient;
    }
    destinationFaceleft
    {
        type            zeroGradient;
    }
    channelWallsleft
    {
        type            zeroGradient;
    }
    leftRightWallleft
    {
        type            cyclicAMI;
    }
    inlet
    {
        type            zeroGradient;
    }

}

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

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.1                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
       leftRightWallsright
    {
        type            cyclicAMI;
    }
    outlet
    {
        type            zeroGradient;
    }
    channelWallsright
    {
        type            fixedValue;
        value           uniform 0;
    }
    destinationFaceright
    {
        type            noSlip;
    }
    sourceFaceright
    {
        type            noSlip;
    }
    sourceFaceleft
    {
        type            noSlip;
    }
    destinationFaceleft
    {
        type            noSlip;
    }
    channelWallsleft
    {
        type            noSlip;
    }
    leftRightWallleft
    {
        type            cyclicAMI;
    }
    inlet
    {
        type            fixedValue;
        value           uniform(1 0 0);
    }
}

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

[RobertHB]

Originally Posted by bshambaugh

I ran the code and I obtained in log.icoFoam: "
"ill defined primitiveEntry starting at keyword 'value' on line 63 and ending at line 69"

Usually a sign that you missed a semicolon somewhere, but i checked your U dict and you didn't.
But on line 63 i find

value           uniform(1 0 0);

so i'm guessing that your simulation might struggle with the missing space between uniform and (1 0 0);


Furthermore, on line 34 you have

value           uniform 0;

which will most likely complain. Use uniform (0 0 0);