[sc369]

i created a interfoam case it did run well
but
i used this case previously that time it worked but now i just replaced the stl files now the blockmesh , surfacefeatureextract, and snappy are running well but when i run decompose par or interfoam command i am getting this error i did looked at the lines but theire isnt any change and whole case is same as previous working case. no change except location in mesh, blockmesh size, and stl files


error
Lenovo-ideapad-520-15IKB:~/Desktop/TESTC$ interFoam
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2306 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : _fbf00d6b-20230626 OPENFOAM=2306 version=2306
Arch : "LSB;label=32;scalar=64"
Exec : interFoam
Date : Mar 07 2024
Time : 12:50:54
Host : sahil-Lenovo-ideapad-520-15IKB
PID : 21665
I/O : uncollated
Case : /home/sahil/Desktop/TESTC
nProcs : 1
trapFpe: Floating point exception trapping enabled (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 5, maxFileModificationPolls 20)
allowSystemOperations : Allowing user-supplied system call operations

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

--> FOAM Warning :
From static Foam::IOstreamOption::compressionType Foam::IOstreamOption::compressionEnum(const Foam::word&, Foam::IOstreamOption::compressionType)
in file db/options/IOstreamOption.C at line 115
Unknown compression specifier 'uncompressed', using compression off
Create mesh for time = 0

Selecting dynamicFvMesh staticFvMesh

PIMPLE: Operating solver in PISO mode

Reading field p_rgh



--> FOAM FATAL IO ERROR: (openfoam-2306)
Cannot find patchField entry for allBoundary

file: 0/p_rgh.boundaryField at line 28 to 49.

From void Foam::GeometricBoundaryField<Type, PatchField, GeoMesh>::readField(const Foam:imensionedField<TypeR, GeoMesh>&, const Foam::dictionary&) [with Type = double; PatchField = Foam::fvPatchField; GeoMesh = Foam::volMesh]
in file ./src/OpenFOAM/lnInclude/GeometricBoundaryField.C at line 177.

FOAM exiting

Lenovo-ideapad-520-15IKB:~/Desktop/TESTC$



please do help in solving this Error if u have any Question u cantact me
Thanks in advance.

[Yann]

Hello,

This is a very common problem, you can use the search function to find posts about similar issues on the forum.

"Cannot find patchField entry for allBoundary" - when setting two inlets in interFoam

Check your mesh and boundary conditions and see which one is wrong.

Regards,
Yann

[sc369]

Originally Posted by Yann

Hello,

This is a very common problem, you can use the search function to find posts about similar issues on the forum.

"Cannot find patchField entry for allBoundary" - when setting two inlets in interFoam

Check your mesh and boundary conditions and see which one is wrong.

Regards,
Yann

Thankyou for this can u please Explain why my other cases are working whereas Everything is same Except cad files

[Yann]

If allBoundary is a patch defined in blockMesh: it got removed while meshing your geometry in your previous meshes but not on this one, because the CAD file is not the same.

I have no idea about what you are meshing and what changed in your CAD files so this is up to you.

Check your mesh in ParaView, load the patches and see what is wrong and why you still have allBoundary patch if this is not supposed to be there anymore.

Yann

[sc369]

Originally Posted by Yann

If allBoundary is a patch defined in blockMesh: it got removed while meshing your geometry in your previous meshes but not on this one, because the CAD file is not the same.

I have no idea about what you are meshing and what changed in your CAD files so this is up to you.

Check your mesh in ParaView, load the patches and see what is wrong and why you still have allBoundary patch if this is not supposed to be there anymore.

Yann

/*--------------------------------*- 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 dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

//These vertices define the block below. It envelopes the stl files. The block can be even bigger than the stl files
//Watch out if the stl files are created in mm or m!

vertices
(
( -5 -4 -1)
( 5 -4 -1)
( 5 6 -1)
( -5 6 -1)
( -5 -4 20)
( 5 -4 20)
( 5 6 20)
( -5 6 20)
);

blocks
(
hex (0 1 2 3 4 5 6 7) (30 30 30) simpleGrading (1 1 1)//coarse grid - we will refine in snappyHexMeshDict
);

edges
(
);

boundary
(
allBoundary//Don't worry about these settings
{
type patch;
faces
(
(3 7 6 2)
(0 4 7 3)
(2 6 5 1)
(1 5 4 0)
(0 3 2 1)
(4 5 6 7)
);
}
);
can you please guide me how to correct it this is my blockmeshdict file it do have allboundary

[Yann]

The blockMesh is not necessarily the issue.

What mesh do you get when you open it in ParaView?
What is the geometry you are trying to mesh?

[sc369]

Originally Posted by Yann

The blockMesh is not necessarily the issue.

What mesh do you get when you open it in ParaView?
What is the geometry you are trying to mesh?

https://drive.google.com/file/d/1-T7...usp=drive_link
here is link to my file
i am Experimenting on Dental cavity for internal flow. i am getting the mesh of internal area as it was required

[Yann]

Alright so in the allBoundary.png file you can see your mesh. the allBoundary patch is in red. Since this is a boundary of your mesh, you need to define boundary condition for this patch in order to be able to run the solver. This is the error message you get (Cannot find patchField entry for allBoundary)

You get this patch because the upper bound of your STL files on the z axis perfectly align with the blocMesh boundary. (blockMesh_and_stl.png)

Now it's up to you to decide how to solve this. If the mesh is ok, you can just define proper boundary conditions for the allBoundary patch.

If allBoundary patch is not supposed to be here, you need to extend the upper bound of your blockMesh so the STL files are fully enclosed in the blockMesh. While meshing snappy with remove all cells around your geometry and you won't have any allBoundary patch left after meshing.

This being said, your STL files are a bit weird:
the straightCase.stl is a closed volume, it is defined in the geometry section of your snappyHexMeshDict but it is not used anywhere so it is useless.

You are actually meshing the inlet.stl, outlet.stl, cavity_wall.stl and needle_wall.stl but these STL do not form a closed volume. (stl_files.stl)
A surface is missing to close the volume so if you extend your blockMesh dimensions you won't get the expected result.

Long story short : you can either add boundary conditions for allBoundary or extend your blockMesh and fix your STL files by adding the missing surface.

Cheers,
Yann

[sc369]

Originally Posted by Yann

Alright so in the allBoundary.png file you can see your mesh. the allBoundary patch is in red. Since this is a boundary of your mesh, you need to define boundary condition for this patch in order to be able to run the solver. This is the error message you get (Cannot find patchField entry for allBoundary)

You get this patch because the upper bound of your STL files on the z axis perfectly align with the blocMesh boundary. (blockMesh_and_stl.png)

Now it's up to you to decide how to solve this. If the mesh is ok, you can just define proper boundary conditions for the allBoundary patch.

If allBoundary patch is not supposed to be here, you need to extend the upper bound of your blockMesh so the STL files are fully enclosed in the blockMesh. While meshing snappy with remove all cells around your geometry and you won't have any allBoundary patch left after meshing.

This being said, your STL files are a bit weird:
the straightCase.stl is a closed volume, it is defined in the geometry section of your snappyHexMeshDict but it is not used anywhere so it is useless.

You are actually meshing the inlet.stl, outlet.stl, cavity_wall.stl and needle_wall.stl but these STL do not form a closed volume. (stl_files.stl)
A surface is missing to close the volume so if you extend your blockMesh dimensions you won't get the expected result.

Long story short : you can either add boundary conditions for allBoundary or extend your blockMesh and fix your STL files by adding the missing surface.

Cheers,
Yann

thankyou so much for resolving this issue