View source for BlockMesh

__FORCETOC__

= Introduction =
<tt>blockMesh</tt> is one of the most basic mesh generators in OpenFOAM. It relies on a single dictionary file <tt>blockMeshDict</tt>, usually placed inside the folders <tt>constant/polyMesh</tt> or <tt>system/</tt>. The latest official documentation on how to use <tt>blockMesh</tt> can be found on the OpenFOAM User Guide and online at the OpenFOAM Foundation website at this page: [http://www.openfoam.org/docs/user/blockMesh.php 5.3 blockMesh]

{{VersionInfo}} {{version1.0}} {{version1.1}} {{version1.2}} {{version1.3}} {{version1.4}} {{version1.5}} {{version1.6}} {{version1.7}} {{version2.0}} {{version2.1}} {{version2.2}} {{version2.3}} {{version1.4-dev}} {{version1.5-dev}} {{version1.6-ext}} {{version3.0-ext}}

Feel free to contribute to this page!


==Synopsis==
blockMesh [OPTIONS]

==Description==
As the name implies, {{tt|blockMesh}} helps the user build the mesh with blocks. It relies on a single dictionary file {{tt|blockMeshDict}}, usually located at {{tt|constant/polyMesh/blockMeshDict}} or {{tt|system/blockMeshDict}}. Inside that dictionary file should be defined:
# all of the reference vertices of mesh;
# all of the building blocks for the mesh, each block composed of:
#* 8 vertices (repeat vertices, for collapsing edges);
#* grading definition;
#* cell count over each major axis;
# optionally, one can assign special edge definitions for specific edges on blocks, such as arcs and splines;
# assign faces of blocks to patch names;
# and finally, be able to define special face merging, but associating/merging patches.

The following options can be used with {{tt|blockMesh}}:

'''-case''' ''DIR''
:Execute the command on the case directory ''DIR''. If not provided, use the current directory.
'''-dict''' ''FILE''
:Read dictionary from specified location.
'''-blockTopology'''
: Write block edges and centres as {{tt|.obj}} files, for visual inspection elsewhere.
'''-noFunctionObjects'''
:Skip the execution of the [[functionObjects]]
'''-region''' ''NAME''
:Generate the mesh only for a specific region (e.g. for multi-region simulations).
'''-help'''
:Display the help and exit

= Tips =
On this chapter are listed links and direct tips on using <tt>snappyHexMesh</tt>.

== Using {{tt|blockMesh}} to export {{tt|blockMeshDict}} to {{tt|.obj}}  ==
Before there were any nice graphical user interfaces for visually designing and inspecting the {{tt|blockMeshDict}} files, {{tt|blockMesh}} can interpret the dictionary file and export it to an {{tt|.obj}} file, which can be opened by any compatible 3D software, such as ParaView, JavaView and so on. There steps are as follows:

# Use the {{tt|-blockTopology}} argument to dump out a {{tt|blockTopology.obj}} file: <bash>blockMesh -blockTopology</bash>
# The vertex numbering in this file is consistent with that of the vertices in the {{tt|blockMeshDict}} file.
# The file {{tt|blockTopology.obj}} can be visualized in the following 3D software:
#* Visualize directly with JavaView;
#* Visualize directly in ParaView or convert the file to VTK if you prefer: <bash>objToVTK blockTopology.obj blockTopology.vtk</bash>
#* Import in Blender.
#* ''(fell free to add more...)''


== Graphical User Interfaces for visualizing and designing {{tt|blockMeshDict}} ==

;{{tt|paraFoam -block}}: Introduced in OpenFOAM 2.0.0, this argument for the {{tt|paraFoam}} script requires that the respective OpenFOAM plugin is built for ParaView. This means that ParaView has to be built from source code or to use the Deb/RPM packages provided by the OpenFOAM Foundation.

;{{tt|blockMesh -blockTopology}}: Already explained in the section [[#Using blockMesh to export blockMeshDict to .obj|Using {{tt|blockMesh}} to export {{tt|blockMeshDict}} to {{tt|.obj}}]]

;{{tt|pyFoamDisplayBlockMesh.py}}: This Python script provides a way to visually inspect the current {{tt|blockMeshDict}} settings in 3D. It is part of [[Contrib/PyFoam|PyFoam]], which relies on VTK and Qt for the graphical interface. For more information, see section [[Contrib/PyFoam#pyFoamDisplayBlockMesh.py|pyFoamDisplayBlockMesh.py]] in the page [[Contrib/PyFoam]].

;SwiftBlock: This is also a Python script, but it's a powerful add-on for Blender, which provides an interactive way to design the {{tt|blockMeshDict}} directly in 3D. For more information, see the respective wiki page: [[Contrib/SwiftBlock]]

;HexBlocker: This is a dedicated application for visually editing in 3D the {{tt|blockMeshDict}} file. For more information, see this forum page: [http://www.cfd-online.com/Forums/openfoam-meshing/114773-hexblocker-gui-blockmeshdict-alpha-release.html HexBlocker a GUI for blockMeshDict, alpha release]

;FreeCAD: If you are looking for out of the box and cross platform solutions, there are attempts to import blockMeshDict topologies into FreeCAD. The other advantage is that it does not require the mesh, so if you have problems with mesh generation it help you to visualize in advance and debug the topology. An early version of the Python script can be found [https://gist.github.com/Foadsf/9ef9975d31bb01fa2bb88b6db7e0bda9 here]. To follow up on this project you may follow [https://forum.freecadweb.org/viewtopic.php?f=37&t=30426 this thread] in FreeCAD forum.

== Calculating the grading ==

There is [[Scripts/blockMesh_grading_calculation|this utility]] here on the Wiki and [http://www.cfd-online.com/Forums/openfoam-meshing-blockmesh/61785-blockmesh-grading-calculator.html this thread with a utility on the MessageBoard].

== Programmatically generating {{tt|blockMeshDict}} files ==
Since the {{tt|blockMeshDict}} files are essentially text files, they can be generated by any means necessary. In this section is addressed the currently known documented ways of using scripts to generate {{tt|blockMeshDict}} files.

; {{tt|#codeStream}}: This is a feature that was introduced in OpenFOAM 2.0.0: [http://openfoam.org/release/2-0-0/run-time-control-code-compilation/ OpenFOAM® v2.0.0: Run-time Control] - Examples:
:* The main tutorial provided in OpenFOAM for this feature in {{tt|blockMeshDict}}: {{tt|$FOAM_TUTORIALS/basic/potentialFoam/cylinder}}

;GNU m4, ''aka'' {{tt|blockMeshDict.m4}}: 
:* The [https://www.gnu.org/software/m4/m4.html GNU m4 (manual)] is a macro processor, which is essentially a simple programming language for calculating values and definitions to be written in the resulting file. In the following wiki page is a good example on this topic: [[HowTo blockMesh with m4]]. For more examples, run in the command line: <bash>find $FOAM_TUTORIALS -name "blockMeshDict.m4"</bash>
:* A report by Erwin Adi Hartono for the [http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2010/ MSc/PhD course in CFD with OpenSource software, 2010] at Chalmers University of Technology:  [http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2010/erwinAdiHartono/erwinAdiHartonoReport.pdf Python Scripting and M4-Scripting for Automatization and Parameterization in OpenFOAM]

;MATLAB:
:* BananaSplit: This is a MATLAB script for generating {{tt|blockMeshDict}} files. For more information, see this forum thread: [http://www.cfd-online.com/Forums/openfoam-meshing/108336-bananasplit-helper-openfoam-blockmesh.html BananaSplit helper for OpenFOAM blockMesh]

; Using Python scripts:
:* Generating a pipe: [http://www.cfd-online.com/Forums/openfoam-meshing-blockmesh/82520-how-create-large-mesh.html#post285979 How to create large Mesh? - post #4]
:* Python library {{tt|ofblockmeshdicthelper}} available at PyPi: [https://pypi.python.org/pypi/ofblockmeshdicthelper ofblockmeshdicthelper]
:* Blog post on how to use {{tt|numpy}} for creating the {{tt|blockMeshDict}} file:  [http://dambreak.blogspot.pt/2013/06/generating-openfoam-mesh-from-point.html Generating an OpenFOAM mesh from a point cloud (x,y,z)]

<br>

== Generating double-graded meshes ==
Although {{tt|blockMesh}} is considerably powerful as it is, the community has provided a modified version named {{tt|blockMeshDG}} for generating double graded meshes, in the sense of having an easy way to define symmetrical geometrical grading. For more information, see the dedicated wiki page: [[Contrib_blockMeshDG|blockMeshDG]]


== Generating multi-graded meshes ==

A new feature was introduced into OpenFOAM 2.3.x, some weeks after the release of 2.3.1, which is the ability to do multi-grading. This was introduced in the commit [https://github.com/OpenFOAM/OpenFOAM-2.3.x/commit/cf370883644ec59782be375041b2434eb3e2c4ed cf370883644e] and is documented in the comment of the commit with the usage instructions. Quoting from said comment:
<pre>
    '''blockMesh: Add support for multi/sectional grading in a block'''

    Consider a block describing a channel with two opposite walls.
    Currently in order to grade the mesh towards the walls and have a
    uniform region in the centre the channel would need to be spit into 3
    blocks.  With the new multi/sectional grading this can be achieved in a
    single block e.g.

    blocks
    (
        hex (0 1 2 3 4 5 6 7) (20 60 20)
        simpleGrading
        (
            1
            ((0.2 0.3 4) (0.6 0.4 1) (0.2 0.3 0.25))
            1
        )
    );

    In this example the block is divided uniformly in the x and z -directions
    and split into three grading sections in the y-direction described by
    three triples:  ((0.2 0.3 4) (0.6 0.4 1) (0.2 0.3 0.25)).  Each of the
    grading sections is described by a triple consisting of the fraction of
    the block, the fraction of the divisions and the grading ratio (size of
    first division/size of last division).  Both the fraction of the block
    and the fraction of the divisions are normalized automatically so they
    can be specified scaled in anyway, e.g. as percentages:

    blocks
    (
        hex (0 1 2 3 4 5 6 7) (20 60 20)
        simpleGrading
        (
            1
            ((2 3 4) (6 4 1) (2 3 0.25))
            1
        )
    );

    and they need not sum to 1 or 100.

    This is very new functionality and not well tested but backward
    compatibility has been well tested so all existing blockMeshDicts should
    parse correctly.
</pre>

If you want to use this feature in older versions of OpenFOAM, follow the instructions given on this forum post: [http://www.cfd-online.com/Forums/openfoam-meshing-blockmesh/70798-blockmesh-double-grading-5.html#post567551 blockMesh with double grading. - post #86]

== Generating meshes with smoothed mesh transitions ==
Sometimes it's necessary to transition between different mesh formats, such as going from a cube-shaped block to a sphere-shaped block. This is where the {{tt|extBlockMesh}} add-on for {{tt|blockMesh}} comes in handy: [http://www.cfd-online.com/Forums/openfoam-meshing/132628-extend-blockmesh-smoothing-capability.html#post484113 Extend blockMesh with smoothing capability]

== Defining cellZones ==
Blocks are assigned to cellZones (which can be used for example to apply fvOptions to a selected region) the name of the cellZone can be specified in the block definition between the vertex numbers and the number of cells in each direction. This information is then used to generate a "cellZones" file in the polyMesh folder:
 ''hex (0 1 2 3 4 5 6 7) myCellZone (20 1 1) simpleGrading (1 1 1)''


[[Category:Mesh generation utilities]]