CFD Online Discussion Forums - createPatch command

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - createPatch command (https://www.cfd-online.com/Forums/openfoam-solving/222440-createpatch-command.html)

createPatch command

Hi, i run with createPatch command and i checked polyMesh boundary file and 0 file. i cannot see any problem.
Could anyoone guide me how to do ?

Thanks everyone who will answer

--> FOAM Warning :
From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam::polyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 473
Removing patchGroup 'wall' which clashes with patch 6 of the same name.
--> FOAM Warning :
From function Foam::labelHashSet Foam::polyBoundaryMesh::patchSet(const Foam::UList<Foam::wordRe>&, bool, bool) const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 804
Cannot find any patch or group names matching cyclic1
--> FOAM Warning :
From function Foam::labelHashSet Foam::polyBoundaryMesh::patchSet(const Foam::UList<Foam::wordRe>&, bool, bool) const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 804
Cannot find any patch or group names matching cyclic2
--> FOAM Warning :
From function Foam::labelHashSet Foam::polyBoundaryMesh::patchSet(const Foam::UList<Foam::wordRe>&, bool, bool) const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 804
Cannot find any patch or group names matching cyclic1
--> FOAM Warning :
From function Foam::labelHashSet Foam::polyBoundaryMesh::patchSet(const Foam::UList<Foam::wordRe>&, bool, bool) const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 804
Cannot find any patch or group names matching cyclic2

From the warning messages, I guess, you've got the syntax of createPatchDict wrong. Apparently, you tried to use the patch name 'wall' twice. Maybe there is already a patch 'wall' in your model. And possibly, you tried to use faceSet names that aren't defined (e.g. in topoSetDict). If you post the file createPatchDict, maybe we'll know more.

thank u for answering.

My createPatch file:

Code:

 /*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.4.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

\*---------------------------------------------------------------------------*/

FoamFile

{

    version     2.0;

    format      ascii;

    class       dictionary;

    object      createPatchDict;

}

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



// Do a synchronisation of coupled points after creation of any patches.

// Note: this does not work with points that are on multiple coupled patches

//       with transformations (i.e. cyclics).

pointSync false;



// Patches to create.

patches

(

    {

        //- Master side patch

        name            periodic1;

        patchInfo

        {

            type            cyclic;

            matchTolerance  0.0001;

            neighbourPatch  periodic2;

           // transform       noOrdering;

             transform translational;

            separationVector (0 -0.032841912 0);

        }

        constructFrom patches;

        patches (cyclic1);

    }



    {

        //- Slave side patch

        name            periodic2;

        patchInfo

        {

            type            cyclic;

            matchTolerance  0.0001;

            neighbourPatch  periodic1;

       //     transform       noOrdering;

         transform translational;

            separationVector (0 0.032841912 0); 

        }

        constructFrom patches;

        patches (cyclic2);

    }



    

    

    {

        //- Master side patch

        name            frontcyc;

        patchInfo

        {

            type            cyclic;

            matchTolerance  0.0001;

            neighbourPatch  backcyc;

           // transform       noOrdering;

            transform translational;

            separationVector (0 0 -0.0005);

        }

        constructFrom patches;

        patches (cyclic1);

    }



    {

        //- Slave side patch

        name            backcyc;

        patchInfo

        {

            type            cyclic;

            matchTolerance  0.0001;

            neighbourPatch  frontcyc;

       //     transform       noOrdering;

 transform translational;

            separationVector (0 0 0.0005);

        }

        constructFrom patches;

        patches (cyclic2);

    }

    

   /* {

        name inlet;

        patchInfo

        {

            type            patch;

        }

        constructFrom set;

        set inletFaces;

    }

    {

        name outlet;

        patchInfo

        {

            type            patch;

        }

        constructFrom set;

        set outletFaces;

    }*/

);



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

I don't understand the warning about patchGroup 'wall'. This name is not used in your createPatchDict. Maybe, you should also check the file /constant/polyMesh/boundary.
The other warnings are about patches to be created from the existing patches 'cyclic1' and 'cyclic2'. I expect, these patches must also be defined in /constant/polyMesh/boundary. If they are not there, createPatch cannot find them.

Hi Mekim, attaching your boundary mesh would help to find the error

thank u for your attention.

my boundary file:

Code:

 FoamFile

{

    version     2.0;

    format      ascii;

    class       polyBoundaryMesh;

    location    "constant/polyMesh";

    object      boundary;

}

         

(

    backcyc

    {

        type patch;

        nFaces 39606;

        startFace 78626;

    }

    periodic1

    {

        type patch;

        nFaces 268;

        startFace 118232;

    }

    periodic2

    {

        type patch;

        nFaces 268;

        startFace 118500;

    }

    frontcyc

    {

        type patch;

        nFaces 39606;

        startFace 118768;

    }

    inlet

    {

        type patch;

        nFaces 147;

        startFace 158374;

    }

    outlet

    {

        type patch;

        nFaces 119;

        startFace 158521;

    }

    wall

    {

        type wall;

        nFaces 370;

        startFace 158640;

    }

)

So, this is your boundary file after running createPatch, is it? It seems fine. Maybe you tried to run createPatch twice? ;)

I solved the problem. I edited the pacthes (..) part.

'edited the patches (..) part' ??

Hi,
I am having the same problem, but I don't understand what you mean when you say you solved the problem. Can you give more detail about what you did with the 'patches (..)' part?

Hi,

I am taking the same problem when I define wedges in my boundry and I can't solve the problem.

Code:

--> FOAM Warning : Creating fvModels from "constant/fvOptions"



Selecting finite volume model type radiation

    Name: radiation

Selecting radiationModel P1

Selecting absorptionEmissionModel greyMeanCombustion

Selecting scatterModel none

Selecting soot model none

--> FOAM Warning :

    From function const Foam::HashTable<Foam::List<int>, Foam::word>& Foam::polyBoundaryMesh::groupPatchIDs() const

    in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 473

    Removing patchGroup 'wall' which clashes with patch 5 of the same name.

--> FOAM Warning : Creating fvConstraints from "constant/fvOptions" rather than system/fvConstraints

No fvConstraints present

Rename group wall to walls.

Allow me.

I had the same. My system/blockMesh showed,

Code:

boundary ( wall { type wall; faces ( (0 1 2 3) (4 5 6 7) ); } )

Changing to

Code:

boundary ( walls { type wall; faces ( (0 1 2 3) (4 5 6 7) ); } )

fixed things. Don't forget to update references to wall in 0/* to walls.

Apologies for the inline format.

BR,

Mark.