[Simjoh]

I'm currently running a case where I use snappyHexMesh to generate my grid. The mesh is all good despite some small deficiencies at corners of my geometry but I can live with those.

I generate my case as the flange tutoríal and after the mesh generation I end up with one addidional boundary in constant/polyMesh/boundary. This extra boundary is the one created by blockMesh.

If I try to run the case as is It complains about the missing BC in the 0 folder for U and p_rgh for the boundary created by blockMesh. In the flange tutorial this boundary is called allBoundary.


The simulation do run if i manually delete the the allBoundary lines in contstant/polyMesh/boundary.

Is there any why to do this from the commandline or any built in openFOAM tools?

[Antimony]

Hi,

In the constant/polyMesh/boundary does the "allBoundary" patch have 0 faces?

If that is the case then you can run createPatch to remove zero-sized patches, though I would expect snappy to have already taken care of that.

Cheers,
Antimony

[Simjoh]

Thanks Antimony for at quick response.

Yes I guess it is zero since I got the nFaces 0;

This was the solution to my problem. There are a lot of complicated examples of createPachDict in the tutorials.
Since my case is simple without any moving parts i used tutorials/incompressible/simpleFoam/rotorDisk/system/createPatchDict. If I use this as is all the paches with zero faces will be removed
For the ones to lazy to find that file I attach the code form that file

 /*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  3.0.1                                 |
|   \\  /    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. An empty patch list just removes patches with zero
// faces from $FOAM_CASE/constant/polyMesh/boundary.
patches
(

);
// ************************************************************************* //

[Antimony]

Hi,

Used the attached as your createPatchDict to remove zero size patches.

Cheers,
Antimony

[erlend_grotle]

This solved my problem nicely. I used the file shown in #3.
Then I copied polyMesh files from 0.01 folder to the constant folder and deleted 0.01.
Nice..:!!

BR
Erlend

[Simjoh]

I'm not familiar with the copy and paste procedure you are doing.
Maybe you could use

createPatch -overwrite