CFD Online Discussion Forums - [snappyHexMesh] SnappyHexMesh Point is not inside Mesh but it is

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

- OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)

- - [snappyHexMesh] SnappyHexMesh Point is not inside Mesh but it is (https://www.cfd-online.com/Forums/openfoam-meshing/61484-snappyhexmesh-point-not-inside-mesh-but.html)

SnappyHexMesh Point is not inside Mesh but it is

Hi everyOne,

maybe this is an easy one. Meshing with snappyHexMesh I sometimes get the error message:

Point (51 35 45) is not inside the mesh or on a face or edge.
Bounding box of the meshhttp://www.cfd-online.com/OpenFOAM_D...lipart/sad.gif-1500 -300 -500) (500 1200 1200)

From function refinementParameters::findCells(const polyMesh&) const
in file autoHexMesh/autoHexMeshDriver/refinementParameters/refinementParameters.C at line 104.

FOAM exiting

it tells me, that the point, that defines the keeping mesh zone, is not inside the initial mesh....but it is. i can try with a whole bunch of other coordinates with the same result (i don't think they all accidentely match a cell-face).

maybe someone of you had the same problem sometime and knows the answer. the case itself is a very simple one. i've already managed to mesh with sHM but this one is bugging me, because there seems no plausible explaination.

hi,

did you find out why this happens? I have the same problem.

They key is in "... or on a face or edge", snappyHexMesh can't have the deciding point lie on a face or edge. Try something like (51.3141592654 35.3141592654 45.3141592654), instead of (51 35 45) - ie. something that is unlikely to come up during the cell divisions.

Cheers
Andrew

I'm also having this problem and increasing the number of deciaml places is not helping. Has anyone found a proper workaround for this?

...and I've just found the problem! Make sure you have defined your bounding box properly, starting with the face at minX then the face at maxX. Don't know if this is properly explaining what the issue was, but this works for me. See below:

vertices
(
( 750 -750 750)
( 750 750 750)
( 750 750 -750)
( 750 -750 -750)
(-750 -750 750)
(-750 750 750)
(-750 750 -750)
(-750 -750 -750)
);
blocks
(
//hex(0 3 2 1 4 7 6 5) (20 20 20) simpleGrading (1 1 1) <--this is wrong
hex (4 7 6 5 0 3 2 1) (20 20 20) simpleGrading (1 1 1) // this is correct
);

Worked perfect, thanks!

The proper way to do it is to set up your blockMesh domain as per section 5.3 in the user guide. You should use the setup in figure 5.5 on page U-142.

right-handed coordinate system x1x2x3
x1 direction described by moving from vertex 0 to vertex 1
x2 direction described by moving from vertex 1 to vertex 2
vertices 0, 1, 2, 3 define the plane x3 = 0
vertex 4 is found by moving by moving from vertex 0 in the x3 direction
vertices 5,6 and 7 are similarly found by moving in the x3 direction from vertices 1,2
and 3 respectively

Quote:

Originally Posted by ziad (Post 273901)

Its works fine (y)

Thank you :)

vertices
(
(48 660 -2015)
(2000 660 -2015)
(2000 3000 -2015)
(48 3000 -2015)
(48 660 4000)
(2000 660 4000)
(2000 3000 4000)
(48 3000 4000)
);

blocks
(
hex (3 2 6 7 0 1 5 4) (20 20 20) simpleGrading (1 1 1)

Same problem I guess tried everything still can't figure it out.

Hi abhinavmohan!

I think that the correct order of the points in blockMeshDict should be:

blocks
(
hex (0 1 2 3 4 5 6 7) (20 20 20) simpleGrading (1 1 1)
);

Hope it helps!

abhinavmohan:

What happened is, you did not form the volume you thought you were forming. Which is why you should run checkMesh on the grid when any tools complain about the mesh. Or even beforehand.

The order of points matters, as illustrated in the user guide, section 5.2, table 5.1, "Vertex, face and edge numbering for cellShapes." But I guess "trying everything" doesn't include reading the manual, huh?

Sometimes it is better to clear the polymesh folder and remesh.

For example, all my definitions were correct, (location in mesh, ordering of blockmesh etc) but was still failing (with the message at the begining of this thread). I then deleted polymesh and remeshed (with exactly the same definitions as before) and it worked correctly. It appears that the old polymesh definitions were retained and not cleared.

Nevertheless, if everything fails, one thing to try is to clear out the polymesh folder and restart the meshing process.

hey,

I have been trying to do https://holzmann-cfd.com/community/t.../suzannes-head example in order to learn how creating geometry using blender / Salome and using it in the OpenFOAM simulation.
I created my own background mesh using Salome by following the tutorial shown in the link and when I try to run the command "mpirun -np 4 snappyHexMesh -parallel -overwrite" I got the following error

Code:

--------------------------------------------------------------------------

WARNING: Linux kernel CMA support was requested via the

btl_vader_single_copy_mechanism MCA variable, but CMA support is

not available due to restrictive ptrace settings.



The vader shared memory BTL will fall back on another single-copy

mechanism if one is available. This may result in lower performance.



  Local host: LAPTOP-BKEON11O

--------------------------------------------------------------------------

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

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

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

|  \\    /   O peration     | Version:  v2006                                 |

|   \\  /    A nd           | Website:  www.openfoam.com                      |

|    \\/     M anipulation  |                                                 |

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

Build  : _b45f8f6f58-20200629 OPENFOAM=2006

Arch   : "LSB;label=32;scalar=64"

Exec   : snappyHexMesh -parallel -overwrite

Date   : Nov 15 2020

Time   : 20:39:29

Host   : LAPTOP-BKEON11O

PID    : 644

I/O    : uncollated

Case   : /home/sam/OpenFOAM/OpenFOAM-v2006/tutorials/susan

nProcs : 4

Hosts  :

(

    (LAPTOP-BKEON11O 4)

)

Pstream initialized with:

    floatTransfer      : 0

    nProcsSimpleSum    : 0

    commsType          : nonBlocking

    polling iterations : 0

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



Create mesh for time = 0



Read mesh in = 0.02 s



Overall mesh bounding box  : (-1 -0.827093 -0.601021) (1 2.36662 0.671601)

Relative tolerance         : 1e-06

Absolute matching distance : 3.97736e-06



Reading refinement surfaces.

Read refinement surfaces in = 0.01 s



Reading refinement shells.

Read refinement shells in = 0 s



Setting refinement level of surface to be consistent with shells.

For geometry suzanne.stl detected 0 uncached triangles out of 12100

For geometry leftears.stl detected 0 uncached triangles out of 1872

For geometry rightears.stl detected 0 uncached triangles out of 1872

Checked shell refinement in = 0.06 s



Reading features.

Read features in = 0 s





Determining initial surface intersections

-----------------------------------------



Edge intersection testing:

    Number of edges             : 78797

    Number of edges to retest   : 0

    Number of intersected edges : 0

Edge intersection testing:

    Number of edges             : 78797

    Number of edges to retest   : 78797

    Number of intersected edges : 26

Calculated surface intersections in = 0.06 s



Initial mesh : cells:25346  faces:78797  points:28200

Cells per refinement level:

    0   25346



Adding patches for surface regions

----------------------------------



Patch Type                Region

----- ----                ------

monkey:



3     wall                monkey



monkeyLBack:



4     wall                monkeyLBack



monkeyRBack:



5     wall                monkeyRBack



Added patches in = 0 s



Edge intersection testing:

    Number of edges             : 78797

    Number of edges to retest   : 0

    Number of intersected edges : 26

Selecting decompositionMethod simple [4]



Refinement phase

----------------



[0]

[0]

[1]

[1]

[1] --> FOAM FATAL ERROR:

[1] Point (1.2 0.1 0) is not inside the mesh or on a face or edge.

Bounding box of the mesh:(-1 -0.827093 -0.601021) (1 2.36662 0.671601)

[2]

[2]

[2] --> FOAM FATAL ERROR:

[2] Point (1.2 0.1 0) is not inside the mesh or on a face or edge.

Bounding box of the mesh:(-1 -0.827093 -0.601021) (1 2.36662 0.671601)

[2]

[2]     From static Foam::labelList Foam::refinementParameters::findCells(bool, const Foam::polyMesh&, const pointField&)

[2]     in file [3]

[3]

[3] --> FOAM FATAL ERROR:

[3] Point (1.2 0.1 0) is not inside the mesh or on a face or edge.

Bounding box of the mesh:(-1 -0.827093 -0.601021) (1 2.36662 0.671601)

[3]

[3]     From static Foam::labelList Foam::refinementParameters::findCells(bool, const Foam::polyMesh&, const pointField&)

[3]     in file snappyHexMeshDriver/refinementParameters/refinementParameters.C at line 241.[0] --> FOAM FATAL ERROR:

[0] Point (1.2 0.1 0) is not inside the mesh or on a face or edge.

Bounding box of the mesh:(-1 -0.827093 -0.601021) (1 2.36662 0.671601)

[0]

[0]     From static Foam::labelList Foam::refinementParameters::findCells(bool, const Foam::polyMesh&, const pointField&)

[0]     in file snappyHexMeshDriver/refinementParameters/refinementParameters.C at line 241.

[0]

FOAM parallel run exiting

[0]

[1]

[1]     From static Foam::labelList Foam::refinementParameters::findCells(bool, const Foam::polyMesh&, const pointField&)

[1]     in file snappyHexMeshDriver/refinementParameters/refinementParameters.C at line 241.

[1]

FOAM parallel run exiting

[1]

snappyHexMeshDriver/refinementParameters/refinementParameters.C at line 241.

[2]

FOAM parallel run exiting

[2]

--------------------------------------------------------------------------

MPI_ABORT was invoked on rank 2 in communicator MPI_COMM_WORLD

with errorcode 1.



NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes.

You may or may not see the output from other processes, depending on

exactly when Open MPI kills them.

--------------------------------------------------------------------------



[3]

FOAM parallel run exiting

[3]

[LAPTOP-BKEON11O:00640] 3 more processes have sent help message help-btl-vader.txt / cma-permission-denied

[LAPTOP-BKEON11O:00640] Set MCA parameter "orte_base_help_aggregate" to 0 to see all help / error messages

[LAPTOP-BKEON11O:00640] 3 more processes have sent help message help-mpi-api.txt / mpi-abort

I created the Suzannes Head inside the box for sure. Then how is that I get this error?:(

and How do I fix it?

Kind regards
vava10

Hi,

Quote:

Point (1.2 0.1 0) is not inside the mesh or on a face or edge.
Bounding box of the mesh:(-1 -0.827093 -0.601021) (1 2.36662 0.671601)

Well, as you can see from the error message the point you have chosen for the "locationInMesh" is clearly outside the bounds of the mesh that OF sees.

A quick fix would be to change your "locationInMesh" point to (0.2 0.1 0) and see if the resulting mesh is the one you want.

Hope this helps.

Cheers,
Antimony

--> FOAM FATAL ERROR: Neither insidePoint/insidePoints nor outsidePoint/outsidePoin

im getting the above error, please help me rectify it. thank you https://drive.google.com/file/d/1y5m...usp=drive_link