[nathanael]

Hello,

For some time I have been working on writing an add-on in blockMesh in order to smooth the mesh.
After compilation of the code located at Github link you simply need to add the following in your blockMeshDict:

smoother
{    
    elemTransformParameter    0.666;
    maxGETMeIter                1000;
    improvementTolerance        1e-4;
    qMeanRelaxationTable        (1 0.25 0.125 0);
    qMinRelaxationTable         (0.1 0.05 0.01 0);
    maxIneffectiveIteration     5;
    
    features
    {
        featureAngle            30;
        minEdgeForFeature       10;
    }
};

Example and explaination are availlable at link to explaination.




I encourage people to suggests improvements and make own versions.

Nathanaël

[nathanael]

I updated the installation instructions :

# If needed source your Open FOAM bashrc
source OpenFOAM/OpenFOAM-2.2.x/etc/bashrc

# Download the extBlockMesh source and move inside downloaded directory
git clone https://github.com/Etudes-NG/extBlockMesh
cd extBlockMesh

# Copy patch in OpenFOAM source and patch it
cp OF-extBlockMesh-2.x.x.patch $WM_PROJECT_DIR
cd $WM_PROJECT_DIR
patch -p1 < OF-extBlockMesh-2.x.x.patch

# Go back in the directory where you download the extBlockMesh source
cd extBlockMesh

# Run the installation script
./Allwmake.sh

# Run extBlockMesh in place of blockMesh

Hope this will help.

[fumiya]

Hi nathanael,

Thank you for sharing the useful tool and pointing out the GETMe smoothing approach.
I'm learning this method from your code and I have one question.

According to the paper(http://cames.ippt.gov.pl/pdf/CAMES_20_1_4.pdf),
the new mesh node positions are calculated using the formula (9).
I think the weighting coefficients are calculated differently in your code.

Could you look at the attached file and answer my question?

Best regards,
Fumiya

[nathanael]

Hi Fumiya

From the same document on page 59 I read:
<Here denotes the index set of the neighbor elements of , i.e., elements, which share at least one node with >
I understand all red cells in your picture.

There is one error in this part of the code, I correct it for the next release, but unfortunately my hard drive crash and I lost all the git history for this project... So I cannot give you the exact location. (Missing divides by the number of cells somewhere).

The next release is ready for public release in a few weeks.
This release gives a lot of improving in term of speed and some extra stuff... I would not say that blockMeshDict become easy to make but at least less to do with complex edges

Best regards,

Nathanaël.

[nathanael]

Oups I was to fast... Yes you are true: I need to compute the weight for the cell and not the point. I will correct that.

[nathanael]

Hello Fumiya,

Here is a comparison between the two algo, colored using skew quality from paraview (lower is better):



For me this is better with old code (avg quality = 0.8904 vs 0.8896, min quality = 0.7429 vs 0.7201).
And a bit faster with old code, no need to store or compute the list of neighboring cells.

What is your opinion? Have you done some test on your side?

Best regards,

Nathanaël.

[GerhardHolzinger]

Hi,

I installed and tested extBlockMesh. Attached you see a simple mesh of a pipe, nothing fancy. I played around with block and vertex arrangement to create a nice mesh. However, without modifying individual cells, you always reach some limit in terms of mesh beauty.

Attached are some pics and the output of checkMesh.

Great tool.

[GerhardHolzinger]

What I understand up to this point, is this is an enhanced version of blockMesh.
Is there a possibility to call the smoothing seperately?

In some cases I do some mesh-magic after blockMesh has finished, e.g. combine mesh regions, partial refinement.
So, I am wondering if it is possible to do the smoothing after this stuff I just descibed.

[fumiya]

Hi nathanael,

Thank you for your test!

I'm considering using your code for mesh morphing operations.
The displacements of the points on the boundaries are prescribed
and the new positions of the interior points are calculated using GETMe algorithm.

Do you think this is a reasonable approach?

Best regards,
Fumiya

[nathanael]

Hi all,

I'm pleased to announce the new release for extBlockMesh!

Major's change:

• Snapping capability.
• Run faster.
• Construct from polymesh, easy to connect with other app.
  

  MeshSmoother meshSmoother(&mesh, &smootherDict);
  meshSmoother.update();

• hexMeshSmoother app added for smoothing of existing mesh.
• Both hexMeshSmoother and extBlockMesh look in system folder for the dictionary "smootherDict" which contain all settings. For explanation about this dictionary see link to explanations.
• No change in OpenFOAM code needed.

Best regards,

Nathanaël.

[nathanael]

Just to show some of the possibilities with a complex block topology:

[waku2005]

Dear all

First of all, great thanks to Nathanael for this useful tool.
I tested the tutorial attached with the latest git ver. of extBlcokMesh, but in difficulty for my own simple test case of the 2-D O-mesh of NACA4 wing section attached.

It seemed to be OK after blockMesh command (checked by checkMesh command and Paraview), the mesh has only 20000 cells.
After that I ran extBlockMesh command but no response returns even after 1 night.
What's wrong with my mesh (blockMeshDict or smootherDict).
Any comments and suggestions are highly appreciated.



Best regards,
waku2005

[nathanael]

Hello Waku2005,

The problem is located in your blockMeshDict, just comment the boundary blade. I don't understand the reason...
After your mesh is smoothed, just change the name of defaultFaces to blade in the file constant/polyMesh/boundary.

Note: your mesh is very stiff for the smoother, I recommand to reduce the transformParameter to 0.02 or less.

Best regards,

Nathanaël.

[waku2005]

Originally Posted by nathanael

Hello Waku2005,

The problem is located in your blockMeshDict, just comment the boundary blade. I don't understand the reason...
After your mesh is smoothed, just change the name of defaultFaces to blade in the file constant/polyMesh/boundary.

Note: your mesh is very stiff for the smoother, I recommand to reduce the transformParameter to 0.02 or less.

Best regards,

Nathanaël.

Dear Nathanaël

Thanks to your suggestion! It works well after I changed the boundary name and reduced the transformParameter to 0.02.

I also found that the convertToMeters parameter in the blockMeshDict affects the smoothing iteration,
i.e., without two changes suggested in your reply, smoothing iteration had successfully continued after I changed the convertToMeters of 1.0 to 0.1 with no change in smootherDict.
I don't know why it works even only the mesh scale was changed.

Best regards,
waku2005

[pad]

Hi,

This looks like a promising tool.

I know of the gridpro2Foam mesh converter but does anyone know if a utility exists that can convert a GridPro topology (*.fra files) to a blockMeshDict file?

[hk318i]

Update: problem solved!

I am trying to use extBlockMesh but I getting the following errors;

when I tried to compile it using OpenFoam 2.2.x, I got an error

SmootherBoundary.h:32:30: fatal error: extendedEdgeMesh.H: No such file or directory
#include "extendedEdgeMesh.H"

Then I tried OpenFoam 2.3.x, I managed to compile it without errors and run the tutorial as well. But, when I checked the points and faces files, I found very strange characters like binary files and I could not view the mesh in paraview.


the beginning of points file

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      binary;
    class       vectorField;
    location    "constant/polyMesh";
    object      points;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


61776
(l/��a@���Pم*��YJH�;f@W�&�
<f@��n$��� 'A,f@i�'�La@[���0��A���Hf@1Y�^L[a@p�l��V���V�Vf@K8^L\�Za@�9�'�w@�$@�cf@�����Ka@P��ٻ�@}ҫpf@nx�0a@�	�� v$@��Q��,f@�!p\a@P� F��*@�
,�P���f@��7�.L`@7�՞G$�'�����f@�S��R`@u�e�������}��f@Wʼ3�U`@™����NL-2d�f@����U`@tØ���?e�L�p�f@4,?��Q`@�����@�3����f@��!��K`@64�$@K;�B�f@`7�H`@��|6�^,@E%�[D�f@���X�_@�^,��Y/ldg@�o
��g@�8�]@^�:�wV@More��î�g@J-I�|�]@��%d�@�����g@��2ab�]@��Cn$@V����g@z<�A�^@Q$Pօ*@�$���g@�6���ea@�@LJ�*������f@�IL�o�a@X��h�$�Nܙ���f@FQ[C��a@�,	:W��Uڲ��f@:�ʆ��a@�k����8�lܕf

[Barlo]

Hi all,
I have just started to use extBlockMesh and I was trying to build a simpleMesh but it seems that I have done some mistakes at some point. Someone knows what is happened?
Thanks in advance,
Lorenzo

[amattosc]

Originally Posted by GerhardHolzinger

Hi,

I installed and tested extBlockMesh. Attached you see a simple mesh of a pipe, nothing fancy. I played around with block and vertex arrangement to create a nice mesh. However, without modifying individual cells, you always reach some limit in terms of mesh beauty.

Attached are some pics and the output of checkMesh.

Great tool.

This looks awesome! I really want to use this add-on to improve my mesh but in what version of openfoam does it work? I tried compiling in foam-extend-3.1 and some libraries were missing.

[hk318i]

I tried it before, it works with OpenFOAM-2.3

[amattosc]

Originally Posted by hk318i

I tried it before, it works with OpenFOAM-2.3

Thank you Hassan! I was able to compile in foam2.3