[blockMesh] merging mesh

cfd1609496 · December 15, 2018, 15:50

doing a structure of "T", i made 4 blocks and with mergepatchPairs done, there is still error exist. The following is my blockMeshdict:

Code:

 /*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.1;

vertices
(
    (1 0 0)
    (2 0 0)
    (2 1 0)
    (1 1 0)
    (1 0 0.1)
    (2 0 0.1)
    (2 1 0.1)
    (1 1 0.1)

    (0 1 0)
    (1 1 0)
    (1 2 0)
    (0 2 0)
    (0 1 0.1)
    (1 1 0.1)
    (1 2 0.1)
    (0 2 0.1)

    (1 1 0)
    (2 1 0)
    (2 2 0)
    (1 2 0)
    (1 1 0.1)
    (2 1 0.1)
    (2 2 0.1)
    (1 2 0.1)
    (2 1 0)
    (3 1 0)
    (3 2 0)
    (2 2 0)
    (2 1 0.1)
    (3 1 0.1)
    (3 2 0.1)
    (2 2 0.1)

);

blocks
(
    hex (0 1 2 3 4 5 6 7) (10 10 1) simpleGrading (1 1 1)
    hex (8 9 10 11 12 13 14 15) (10 10 1) simpleGrading (1 1 1)
    hex (16 17 18 19 20 21 22 23) (10 10 1) simpleGrading (1 1 1)
    hex (24 25 26 27 28 29 30 31) (10 10 1) simpleGrading (1 1 1)

);


edges
(
);

patches
(

patch i1

(
(3 7 6 2)
)

patch i2

(
(16 20 21 17)
)


patch i3

(
(9 13 14 10)
)


patch i4

(
(19 23 20 16)
)

patch i5

(
(18 22 21 17)
)


patch i6

(
(27 31 28 24)
)


);

mergePatchPairs
(
(i1 i2)
(i3 i4)
(i5 i6)
);

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

And the outcome after "Creating merge patch pairs

Code:

Adding point and face zones
Creating attachPolyTopoChanger"
was:
--> FOAM FATAL ERROR:
Face 730 reduced to less than 3 points.  Topological/cutting error B.
Old face: 2(484 605) new face: 2(252 373)

    From function void Foam::slidingInterface::coupleInterface(Foam::polyTopoChange&) const
    in file slidingInterface/coupleSlidingInterface.C at line 1768.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::slidingInterface::coupleInterface(Foam::polyTopoChange&) const at ??:?
#3  Foam::slidingInterface::setRefinement(Foam::polyTopoChange&) const at ??:?
#4  Foam::polyTopoChanger::topoChangeRequest() const at ??:?
#5  Foam::polyTopoChanger::changeMesh(bool, bool, bool, bool) at ??:?
#6  Foam::attachPolyTopoChanger::attach(bool) at ??:?
#7  ? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/blockMesh"
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  ? in "/opt/openfoam6/platforms/linux64GccDPInt32Opt/bin/blockMesh"
Aborted (core dumped)

Is there a need to use stitchMesh or any other things i should look out?
Thanks and appreciate your time.

Sincerely,
yh

wyldckat · December 30, 2018, 14:11

Quick answer: I came here following a PM you sent me, from which I'll also quote part of it here:

Quote:

Originally Posted by cfd1609496

I want to complete and 'I' blocks with 7 blocks separately, but there's always error occur at merging 6th block. Would be grateful if u kindly help check my blockMeshDict:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.1;

vertices
(
   (1 0 0) //bottom mid
    (2 0 0)
    (2 5 0)
    (1 5 0)
    (1 0 8)
    (2 0 8)
    (2 5 8)
    (1 5 8)

    (1 5 0) //mid
    (2 5 0)
    (2 25 0)
    (1 25 0)
    (1 5 8)
    (2 5 8)
    (2 25 8)
    (1 25 8)

    (1 25 0) //upper mid
    (2 25 0)
    (2 30 0)
    (1 30 0)
(1 25 8)
    (2 25 8)
    (2 30 8)
    (1 30 8)

    (0 0 0) //bottom left
    (1 0 0)
    (1 5 0)
    (0 5 0)
    (0 0 8)
    (1 0 8)
    (1 5 8)
    (0 5 8)

    (2 0 0) //bottom right
    (3 0 0)
    (3 5 0)
    (2 5 0)
    (2 0 8)
    (3 0 8)
    (3 5 8)
    (2 5 8)

    (0 25 0) //upper left
    (1 25 0)
    (1 30 0)
    (0 30 0)
    (0 25 8)
    (1 25 8)
    (1 30 8)
    (0 30 8)


);

blocks
(
        hex (0 1 2 3 4 5 6 7) (6 2 6) simpleGrading (1 1 1)
        hex (8 9 10 11 12 13 14 15) (6 8 6) simpleGrading (1 1 1)
        hex (16 17 18 19 20 21 22 23) (6 2 6) simpleGrading (1 1 1)
        hex (24 25 26 27 28 29 30 31) (6 2 6) simpleGrading (1 1 1)
        hex (32 33 34 35 36 37 38 39) (6 2 6) simpleGrading (1 1 1)
        hex (40 41 42 43 44 45 46 47) (6 2 6) simpleGrading (1 1 1)

);

edges
(
);

boundary
(

);

patches
(
patch i1
(
(3 7 6 2)
)

patch i2
(
(8 12 13 9)
)

patch i3
(
(11 15 14 10)
)

patch i4
(
(16 20 21 17)
)

patch i5
(
(0 4 7 3)
)

patch i6
(
(25 29 30 26)
)

patch i7
(
(1 5 6 2)
)

patch i8
(
(32 36 39 35)
)

patch i9
(
(16 20 23 19)
)

patch i10
(
(41 45 46 42)
)

);

mergePatchPairs
(
(i1 i2)
(i3 i4)
(i5 i6)
(i7 i8)
(i9 i10)
);

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

Regarding the first mesh you posted on this thread, the way to diagnose this is to run the following command within the case folder:

Code:

paraFoam -block

This will reveal that one of the problems is related to the fact that there are duplicated vertices, which means that blockMesh is not sure how the faces should connect to each other. It should only have 20 vertices in total, but instead there are 32 vertices.

As for the second mesh, namely the one you sent me via PM, it's the same problem: there are duplicated vertices.

There is a tutorial case in OpenFOAM that demonstrates how a T shape should be meshed, it's the tutorial case "incompressible/pimpleFoam/RAS/TJunction".

cfd1609496 · December 30, 2018, 17:01

Hi, Thanks for the reply.
I try with the multiple vertices definition from this 2nd post in this blog :
https://www.cfd-online.com/Forums/op...9-21-20-a.html

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices 
(
(0 0 0) //a
(2 0 0)
(2 1 0)
(0 1 0)
(0 0 1)
(2 0 1)
(2 1 1)
(0 1 1)
(0 1 0) //b
(2 1 0)
(2 2 0)
(0 2 0)
(0 1 1)
(2 1 1)
(2 2 1)
(0 2 1)
(2 1 0) //c
(3 1 0)
(3 2 0)
(2 2 0)
(2 1 1)
(3 1 1)
(3 2 1)
(2 2 1)
(3 1 0) //d
(5 1 0)
(5 2 0)
(3 2 0)
(3 1 1)
(5 1 1)
(5 2 1)
(3 2 1)
(3 0 0) //e
(5 0 0)
(5 1 0)
(3 1 0)
(3 0 1)
(5 0 1)
(5 1 1)
(3 1 1)

);

blocks 
(
hex (0 1 2 3 4 5 6 7) (10 4 4) simpleGrading (1 1 1) 
hex (8 9 10 11 12 13 14 15) (10 4 4) simpleGrading (1 1 1)
hex (16 17 18 19 20 21 22 23) (5 4 4) simpleGrading (1 1 1)
hex (24 25 26 27 28 29 30 31) (10 4 4) simpleGrading (1 1 1)
hex (32 33 34 35 36 37 38 39) (10 4 4) simpleGrading (1 1 1)
);

edges 
(
);

patches 
(
patch inlet 
(
(0 4 7 3)
(8 12 15 11)

)
patch outlet 
(
(25 26 30 29)
(33 34 38 37)

)
wall upper 
(
(11 15 14 10)
(19 23 22 18)
(27 31 30 26) 
)
wall lower 
(
(0 1 5 4)
(1 2 6 5)
(16 17 21 20)
(32 33 37 36)
(32 36 39 35)

)
wall front 
(
(4 5 6 7)
(12 13 14 15)
(20 21 22 23)
(28 29 30 31)
(36 37 38 39)
)
wall back 
(
(0 3 2 1)
(8 11 10 9)
(16 19 18 17)
(24 27 26 25)
(32 35 34 33)
)

patch i1
(    
(3 7 6 2)
) 

patch i2
(
(8 9 13 12)
)

patch i3
(
(9 10 14 13) 
)

patch i4
(
(16 20 23 19) 
)

patch i5
(
(17 18 22 21) 
)

patch i6
(
(24 28 31 27) 
)

patch i7
(
(24 25 29 28)
)

patch i8
(
(35 39 38 34)
)

);

mergePatchPairs
(
(i2 i1)
(i3 i4)
(i6 i5)
(i7 i8)
);

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

Is there any restriction or guide following this method?
I will try with the non-repeating vertices... thank you

many thanks,
yh

cfd1609496 · January 1, 2019, 06:46

well i made a few blockMeshdict and still unable to make a ''I'' shaped blocks (comprises of 7 separate blocks)

looking from tutorial case: "incompressible/pimpleFoam/RAS/TJunction", the blockMeshdict doesn't have mergePatchpairs needed, but the mesh are well presented and in smooth transition.

1.i tried with this method, no duplicating vertices definition:

Code:

vertices
(
        (0.0 0.0 0.0)   //bottom
        (0.4 0.0 0.0)
        (0.5 0.0 0.0)
        (0.9 0.0 0.0)

        (0.9 0.75 0.0)  //bottom mid
        (0.5 0.75 0.0)
        (0.4 0.75 0.0)
        (0.0 0.75 0.0)

        (0.0 2.25 0.0)  //upper mid
        (0.4 2.25 0.0)
        (0.5 2.25 0.0)
        (0.9 2.25 0.0)

        (0.9 3.0 0.0)   //top
        (0.5 3.0 0.0)
        (0.4 3.0 0.0)
        (0.0 3.0 0.0)

//Z
        (0.0 0.0 0.7)   //bottom
        (0.4 0.0 0.7)
        (0.5 0.0 0.7)
        (0.9 0.0 0.7)

        (0.9 0.75 0.7)  //bottom mid
        (0.5 0.75 0.7)
        (0.4 0.75 0.7)
        (0.0 0.75 0.7)

        (0.0 2.25 0.7)  //upper mid
        (0.4 2.25 0.7)
        (0.5 2.25 0.7)
        (0.9 2.25 0.7)

        (0.9 3.0 0.7)   //top
        (0.5 3.0 0.7)
        (0.4 3.0 0.7)
        (0.0 3.0 0.7)

testing with only two block bottom:

Code:

 blocks
(
        hex (0 1 6 7 16 17 22 23) (2 2 2) simpleGrading (1 1 1)
        hex (1 2 5 6 17 18 21 22) (8 8 8) simpleGrading (1 1 1)
);

error outcome:

Code:

 --> FOAM FATAL ERROR:
Inconsistent number of faces between block pair 0 and 1

    From function void Foam::blockMesh::calcMergeInfo()
    in file blockMesh/blockMeshMerge.C at line 221.

FOAM exiting

any idea and suggestion for the above case?? much appreciated

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

2.and i come up with another definition, learned from this 2nd post in this website: https://www.cfd-online.com/Forums/op...9-21-20-a.html

extracting important part:

Code:

vertices 
(
(0 0 0) //a
(2 0 0)
(2 1 0)
(0 1 0)
(0 0 1)
(2 0 1)
(2 1 1)
(0 1 1)
(0 1 0) //b
(2 1 0)
(2 2 0)
(0 2 0)
(0 1 1)
(2 1 1)
(2 2 1)
(0 2 1)
(2 1 0) //c
(3 1 0)
(3 2 0)
(2 2 0)
(2 1 1)
(3 1 1)
(3 2 1)
(2 2 1)
(3 1 0) //d
(5 1 0)
(5 2 0)
(3 2 0)
(3 1 1)
(5 1 1)
(5 2 1)
(3 2 1)
(3 0 0) //e
(5 0 0)
(5 1 0)
(3 1 0)
(3 0 1)
(5 0 1)
(5 1 1)
(3 1 1)

);

blocks 
(
hex (0 1 2 3 4 5 6 7) (10 4 4) simpleGrading (1 1 1) 
hex (8 9 10 11 12 13 14 15) (10 4 4) simpleGrading (1 1 1)
hex (16 17 18 19 20 21 22 23) (5 4 4) simpleGrading (1 1 1)
hex (24 25 26 27 28 29 30 31) (10 4 4) simpleGrading (1 1 1)
hex (32 33 34 35 36 37 38 39) (10 4 4) simpleGrading (1 1 1)
);


patches
(

patch i1
(    
(3 7 6 2)
) 

patch i2
(
(8 9 13 12)
)

patch i3
(
(9 10 14 13) 
)

patch i4
(
(16 20 23 19) 
)

patch i5
(
(17 18 22 21) 
)

patch i6
(
(24 28 31 27) 
)

patch i7
(
(24 25 29 28)
)

patch i8
(
(35 39 38 34)
)

);

mergePatchPairs
(
(i2 i1)
(i3 i4)
(i6 i5)
(i7 i8)
);

so i come up with my version :

Code:

   vertices
(
    (0.4 0 0) //bottom mid
    (0.5 0 0)
    (0.5 0.75 0)
    (0.4 0.75 0)
    (0.4 0 8)
    (0.5 0 8)
    (0.5 0.75 8)
    (0.4 0.75 8)

    (0.4 0.75 0) //mid
    (0.5 0.75 0)
    (0.5 2.25 0)
    (0.4 2.25 0)

    (0.4 0.75 8)
    (0.5 0.75 8)
    (0.5 2.25 8)
    (0.4 2.25 8)

    (0.4 2.25 0) //upper mid
    (0.5 2.25 0)
    (0.5 3 0)
    (0.4 3 0)
    (0.4 2.25 8)
    (0.5 2.25 8)
    (0.5 3 8)
    (0.4 3 8)

    (0 0 0) //bottom left
    (0.4 0 0)
    (0.4 0.75 0)
    (0 0.75 0)
    (0 0 8)
    (0.4 0 8)
    (0.4 0.75 8)
    (0 0.75 8)

    (0.5 0 0) //bottom right
    (0.9 0 0)
    (0.9 0.75 0)
    (0.5 0.75 0)
    (0.5 0 8)
    (0.9 0 8)
    (0.9 0.75 8)
    (0.5 0.75 8)

    (0.5 2.25 0) //upper right
    (0.9 2.25 0)
    (0.9 3 0)
    (0.5 3 0)
    (0.5 2.25 8)
    (0.9 2.25 8)
    (0.9 3 8)
    (0.5 3 8)


);


blocks
(
        hex (0 1 2 3 4 5 6 7) (6 2 6) simpleGrading (1 1 1)
        hex (8 9 10 11 12 13 14 15) (6 8 6) simpleGrading (1 1 1)
        hex (16 17 18 19 20 21 22 23) (18 2 6) simpleGrading (1 1 1)
        hex (24 25 26 27 28 29 30 31) (6 8 6) simpleGrading (1 1 1)
        hex (32 33 34 35 36 37 38 39) (6 8 6) simpleGrading (1 1 1)
        hex (40 41 42 43 44 45 46 47) (6 8 6) simpleGrading (1 1 1)

);

patch i1
(
(3 7 6 2)
)

patch i2
(
(8 12 13 9)
)

patch i3
(
(11 15 14 10)
)

patch i4
(
(16 20 21 17)
)



patch i5
(
(25 29 30 26)
)

patch i6
(
(0 4 7 3)
)

patch i7
(
(1 5 6 2)
)

patch i8
(
(32 36 39 35)
)

patch i9
(
(17 21 22 18)
)

patch i10
(
(40 44 47 43)
)

);

mergePatchPairs
(
(i1 i2)
(i3 i4)
(i6 i5)
(i7 i8)
(i9 i10)
);

Error outcomes:

Code:

--> FOAM FATAL ERROR:
Face 1028 reduced to less than 3 points.  Topological/cutting error A.
Old face: 2(739 738) new face: 2(739 738)

    From function void Foam::slidingInterface::coupleInterface(Foam::polyTopoChange&) const
    in file slidingInterface/coupleSlidingInterface.C at line 1461.

FOAM aborting

theres no problem in creating the blocks until, always the i9 and i10, no matter what orientation i tried before...is there any rules i missed out in defining blocks?
any suggestion or idea for the block?
Im new to OpenFOAM and wish to learn from anyone, thank you for your patience...sorry for long winding messages

wyldckat · January 1, 2019, 17:19

Quick answers:
Regarding the first block mesh, here you only have 2 blocks and no duplicate vertices, you have to use the following block resolution:

Code:

blocks
(
        hex (0 1 6 7 16 17 22 23) (2 2 2) simpleGrading (1 1 1)
        hex (1 2 5 6 17 18 21 22) (8 2 2) simpleGrading (1 1 1)
);

The reason for this is because blockMesh does not support mesh refinement.

As for the second block mesh, the problem is that it looks like you are trying to do something that blockMesh was not designed to be used for.

----

The problem here is that you're asking how to make something work, without explaining what you are trying to do.
What came to my mind for an analogy, was that it seemed like you are trying to attach 4 wheels to a rocket and expect it to behave as a motorbike

but instead, you are getting a rocket that wobbles until it hits a wall... although perhaps your original intent was to have a fast motorbike and not a rocket with wheels...

If you are trying to create a mesh that has blocks that move along a side of a patch, then the tutorial case "incompressible/pimpleFoam/RAS/oscillatingInletACMI2D" comes to mind, where they did create 2 independent blocks, but do not have duplicate vertices. And there was no need to use "mergePairs", because they are not meant to be merged in this example.

On the other hand, if you are trying to create blocks with different levels of resolution, then you must first have a consistent mesh resolution between blocks and in another step, use topoSet+refineMesh to do the additional increase in refinement. The tutorial case "mesh/refineMesh/refineFieldDirs" has an advanced example of this being done.

cfd1609496 · January 1, 2019, 18:31

Quote:

Originally Posted by wyldckat

Quick answers:
Regarding the first block mesh, here you only have 2 blocks and no duplicate vertices, you have to use the following block resolution:

Code:

blocks
(
        hex (0 1 6 7 16 17 22 23) (2 2 2) simpleGrading (1 1 1)
        hex (1 2 5 6 17 18 21 22) (8 2 2) simpleGrading (1 1 1)
);

The reason for this is because blockMesh does not support mesh refinement.

As for the second block mesh, the problem is that it looks like you are trying to do something that blockMesh was not designed to be used for.

----

The problem here is that you're asking how to make something work, without explaining what you are trying to do.
What came to my mind for an analogy, was that it seemed like you are trying to attach 4 wheels to a rocket and expect it to behave as a motorbike

but instead, you are getting a rocket that wobbles until it hits a wall... although perhaps your original intent was to have a fast motorbike and not a rocket with wheels...

If you are trying to create a mesh that has blocks that move along a side of a patch, then the tutorial case "incompressible/pimpleFoam/RAS/oscillatingInletACMI2D" comes to mind, where they did create 2 independent blocks, but do not have duplicate vertices. And there was no need to use "mergePairs", because they are not meant to be merged in this example.

On the other hand, if you are trying to create blocks with different levels of resolution, then you must first have a consistent mesh resolution between blocks and in another step, use topoSet+refineMesh to do the additional increase in refinement. The tutorial case "mesh/refineMesh/refineFieldDirs" has an advanced example of this being done.

Thank you so much bruno. Thanks with the explanation and the tutorial given. Very appreciate.

Im curious tho, why does the 2nd post in this website: FATAL ERROR: face 6 in patch 2 does not have neighbour cell face: 4(8 9 21 20)
fails for my case?

anyway, thank you one more time for solving the first block mesh.

wyldckat · January 2, 2019, 19:30

Quote:

Originally Posted by cfd1609496

Im curious tho, why does the 2nd post in this website: FATAL ERROR: face 6 in patch 2 does not have neighbour cell face: 4(8 9 21 20)
fails for my case?

My guess is that the solution given in that post #2 required the mesh blocks to have the same mesh resolution, while your mesh the blocks did not have the same resolution.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] Add Mesh Layers doesnt work on the whole surface	Kryo	OpenFOAM Meshing & Mesh Conversion	13	February 17, 2022 07:34
[snappyHexMesh] Creating multiple multiple cell zones with snappyHexMesh - a newbie in deep water!	divergence	OpenFOAM Meshing & Mesh Conversion	0	January 23, 2019 04:17
[snappyHexMesh] SnappyHexMesh no layers and no decent mesh for complex geometry	pizzaspinate	OpenFOAM Meshing & Mesh Conversion	1	February 25, 2015 07:05
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation	tommymoose	ANSYS Meshing & Geometry	48	April 15, 2013 04:24
[snappyHexMesh] Layers:problem with curvature	giulio.topazio	OpenFOAM Meshing & Mesh Conversion	10	August 22, 2012 09:03

January 1, 2019, 17:19		#5
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,975 Blog Entries: 45 Rep Power: 128	Quick answers: Regarding the first block mesh, here you only have 2 blocks and no duplicate vertices, you have to use the following block resolution: Code: blocks ( hex (0 1 6 7 16 17 22 23) (2 2 2) simpleGrading (1 1 1) hex (1 2 5 6 17 18 21 22) (8 2 2) simpleGrading (1 1 1) ); The reason for this is because blockMesh does not support mesh refinement. As for the second block mesh, the problem is that it looks like you are trying to do something that blockMesh was not designed to be used for. ---- The problem here is that you're asking how to make something work, without explaining what you are trying to do. What came to my mind for an analogy, was that it seemed like you are trying to attach 4 wheels to a rocket and expect it to behave as a motorbike but instead, you are getting a rocket that wobbles until it hits a wall... although perhaps your original intent was to have a fast motorbike and not a rocket with wheels... If you are trying to create a mesh that has blocks that move along a side of a patch, then the tutorial case "incompressible/pimpleFoam/RAS/oscillatingInletACMI2D" comes to mind, where they did create 2 independent blocks, but do not have duplicate vertices. And there was no need to use "mergePairs", because they are not meant to be merged in this example. On the other hand, if you are trying to create blocks with different levels of resolution, then you must first have a consistent mesh resolution between blocks and in another step, use topoSet+refineMesh to do the additional increase in refinement. The tutorial case "mesh/refineMesh/refineFieldDirs" has an advanced example of this being done. cfd1609496 likes this. __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM Last edited by wyldckat; January 1, 2019 at 17:20. Reason: added a bit more to the analogy...