[mekim]

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:olyBoundaryMesh::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:olyBoundaryMesh:atchSet(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:olyBoundaryMesh:atchSet(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:olyBoundaryMesh:atchSet(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:olyBoundaryMesh:atchSet(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

[ingraban]

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.

[mekim]

thank u for answering.

My createPatch file:

 /*--------------------------------*- 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;
    }*/
);

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

[ingraban]

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.

[Krao]

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

[mekim]

thank u for your attention.



my boundary file:

 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;
    }
)

[ingraban]

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

[mekim]

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

[boffin5]

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?

[evrenykn]

Hi,

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

--> 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

[anothr_acc]

Allow me.

I had the same. My system/blockMesh showed,

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

Changing to

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.