[joshmccraney]

Hello

When I run setFields I get the error:

--> FOAM FATAL IO ERROR:
Cannot find patchField entry for tank_patch20083

file: /home/josh/Desktop/cases/ICF4/full/case/0/alpha.water.boundaryField from line 26 to line 43.

Prior to this error, I first run snappyHexMesh, which runs error free. Then the issue shouldn't be meshing. Many of these forums suggest this error should be a syntax error. However, I cannot find it. Here's my setFieldsDict

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  6.0                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
    volScalarFieldValue alpha.water 0//only air in the domain
);

regions
(
    boxToCell
    {
        box (0 2 0) (1 5 10);
        fieldValues
        (
            volScalarFieldValue alpha.water 1//we set our block of water into the domain
        );
    }
);


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

and here is my alpha.water

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  4.0                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];//kg m s K mol A cd

internalField   uniform 0;//initially air in the entire domain - we will change that with setFields!

boundaryField
{

    lid
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }

    outlet
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }

    tank
    {
        type            constantAlphaContactAngle;
	theta0		0;
	limit		gradient;
	value		uniform 0;
    }
}

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

Shouldn't the error be in one of these two files? You're help is greatly appreciated!

[Yann]

Hello Josh,

setFields is throwing an error because there is a patch named "tank_patch20083" in the mesh, and there is no boundary condition defined in the alpha.water file for this patch.

You can check what are the patches in your domain in the constant/polyMesh/boundary file :

• at the root of your case if you meshed in serial
• in one of the processor* directories if you meshed in parallel

Another solution is to load your mesh in paraView and check the "Mesh Regions" panel to see the patches list and load the ones you want to see.


Cheers,
Yann

[joshmccraney]

Originally Posted by Yann

Hello Josh,

setFields is throwing an error because there is a patch named "tank_patch20083" in the mesh, and there is no boundary condition defined in the alpha.water file for this patch.

You can check what are the patches in your domain in the constant/polyMesh/boundary file :

• at the root of your case if you meshed in serial
• in one of the processor* directories if you meshed in parallel

Another solution is to load your mesh in paraView and check the "Mesh Regions" panel to see the patches list and load the ones you want to see.


Cheers,
Yann

Wow thanks! I would never have thought to check here! Fort some reason SHM appended all BCs with "_patch20083", which was evidenced in the constant/polyMesh/boundary file. This was different than those listed in the /0 folder. Thanks again Yann!

[Yann]

You're welcome, I'm glad I could help.


The name "patch20083" is probably coming from your STL file. If this is an ASCII STL, you can open it in a text editor and search for the "solid" keyword. Next to "solid", you will see the name(s) of the surface(s) contained in the file (probably coming from the CAD tool you used to create the geometry)


SHM will read the STL file, use the name you provide (tank) and append the surface names contained in the STL file to it (tank_patch20083) which allows to differentiate surfaces in order to use different surface refinement, patch types or layers specifications for each surface.



Cheers,
Yann