CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)
-   -   [blockMesh] about Hex at blockMeshDict (https://www.cfd-online.com/Forums/openfoam-meshing/199514-about-hex-blockmeshdict.html)

arisna March 7, 2018 20:33
about Hex at blockMeshDict
 
Hello everyone,
Could you explain to me about hex ?
for instance :
blocks
(
hex (0 1 5 4 12 13 17 16) (23 8 1) simpleGrading (1 1 1)
hex (2 3 7 6 14 15 19 18) (19 8 1) simpleGrading (1 1 1)
...
I dont know about (23 8 1), do you know?
please tell me,
thank you!:)

Antimony March 7, 2018 21:40
Hi,

(23 8 1) in this case means 23 cells in the first direction (x or x1, however you want to call it), 8 cells in the second direction (y or x2) and 1 cell in the third direction (z or x3)

You can find the details here: https://cfd.direct/openfoam/user-guide/blockmesh/

Cheers,
Antimony

arisna March 8, 2018 05:48
Thank you for your explain.
oh i see, that is to get the grid in 1 box or 1 volume ?

best,
arisna

Quote:
Originally Posted by Antimony (Post 684309)
Hi,

(23 8 1) in this case means 23 cells in the first direction (x or x1, however you want to call it), 8 cells in the second direction (y or x2) and 1 cell in the third direction (z or x3)

You can find the details here: https://cfd.direct/openfoam/user-guide/blockmesh/

Cheers,
Antimony

aow May 31, 2018 22:36
Those 3 numbers of cells in the x, y, and z directions only apply to a single hex. In your example, you have 2 hexes with each one having the same numbers of cells in the y and z directions, but different numbers of cells in the x direction. You would want the y and z cell numbers to be the same if you intended to connect the two hexes as a single mesh object. This approach is called face matching with the alternative being face merging; however, without seeing the rest of your blockMeshDict it is impossible to tell if this is the case. If you have more questions, you should post the entire blockMeshDict in a code block so it's easy to read.

ceren August 31, 2018 02:41
flow on the sharp crested triangle weir
 
http://file:///home/ceren/%C4%B0ndirilenler/images.pngi have a triangle weir. i am trying execute blockmeshdict. this is 3D. i cant do that unfortunately.
have you done it before or like this?

i need guidance.. :confused:
https://www.cfd-online.com/Forums/da...BJRU5ErkJggg==
https://swmm5.org/2016/09/04/weir-ba...-and-infoswmm/https://swmm5.org/2016/09/04/weir-background-equations-for-swmm5-and-infoswmm/
https://www.cfd-online.com/Forums/da...BJRU5ErkJggg==

aow August 31, 2018 15:03
Hi Ceren,

Can you post the details of your geometry and the blockMeshDict that you attempted to use? Then I can try to help you.

As an initial suggestion though, if you want to make a triangular shaped hex region, you need to collapse nodes on top of each other so that 2 pairs of nodes overlap. This is demonstrated in the OpenFOAM User Guide (see image below).

https://cdn.cfd.direct/docs/user-gui...g/user394x.png

Your blockMeshDict entries for such a hex would be something like...

hex (0 1 2 3 4 5 5 4)

and the "collapsed" patch has an area of zero, which means you should give it the empty boundary condition for files in your 0 directory. The patches describing the hex faces should be something like...

(0 1 2 3)
(1 2 5 5)
(0 3 4 4)
(0 1 5 4)
(2 5 4 3)
(4 5 5 4)

A more complete description can be found at...

https://cfd.direct/openfoam/user-guide/v6-blockmesh/

...and looking at section 5.3.5 Creating blocks with fewer than 8 vertices.

Best,

Andrew

aow August 31, 2018 15:18
Also, it might make some sense to just make a large rectangular channel using blockMesh and then import an .stl surface file that has your weir geometry using snappyHexMesh. I had forgotten what a triangle weir looks like and it might be a bit annoying to do using blockMesh alone.

You can make a 3D solid in a program like Autodesk's Inventor and then export it as an .stl file (stereolithography file, which makes a surface out of triangles using unit normal vectors and the coordinates of the triangle corner points). However, before using snappyHexMesh, you would need to extract data from the .stl file using the surfaceFeatureExtract command. Also, your .stl file would need to be placed in <yourCaseDirectory>/constant/trisurface and then you need surfaceFeatureExtractDict in <yourCaseDirectory>/system along with all of the other necessary files.

Then you can build the case with the following commands...

blockMesh
surfaceFeatureExtract
snappyHexMesh
setFields

If your model is very complex in terms of the amount cells you want to use or you want to refine certain regions a lot, then you can run snappyHexMesh in parallel as follows...

decomposePar -copyZero
mpirun -np <numberOfProcessors> snappyHexMesh -parallel
reconstructParMesh -mergeTol 1e-06 -time <lastestTime>
reconstructPar -time <latestTime>

In the above commands, "latestTime" = (number of snappyHexMesh operations)*(time step from controlDict). The 3 possible snappyHexMesh operations are "castellatedMesh", "snap", and "addLayers", which are specified to be either true or false at the beginning of snappyHexMeshDict. The number of these operations that are set to be true is the amount to use when determining "latestTime".

Good luck!

ceren September 1, 2018 04:26
https://swmm5.files.wordpress.com/2016/09/image0096.jpg


hi Andrew,



thank you for your answer. i tried adding picture. i am checking over your writing. I hope I can solve this problem.



thanks again.
ceren

aow September 17, 2018 21:00
Triangular Weir Example
 
1 Attachment(s)
Hey Ceren,

I had a chance to look over the triangular weir problem a bit more and make a demonstration of how to execute the suggestions I gave in my previous post. I attached the case directory I created so you can directly see everything discussed below.

I used Autodesk's Inventor to draw the triangular weir shape with lines to create a closed shape outline and then extruded this shape as a 3D solid. Next I used the export option to save the model as an .stl file, which is how it should be saved for use with OpenFOAM. The image below illustrates the result of these steps.

Triangle Weir Outline with Extruded 3D Solid:

https://i.imgur.com/ArvAVrY.png

To create this example, the weirOverflow tutorial, for which the path should be something like ./OpenFOAM-x.x/tutorials/multiphase/interFoam/RAS/weirOverflow, where x.x is the version number, was copied and heavily modified to create what I hope is a reasonably straightforward example.

In the constant directory, a directory named triSurface was added. Then the weir .stl file, TriangleWeir.stl, was placed in the triSurface directory. Additionally, the gravity file g was adjusted to be (0 0 -9.81) so that the acceleration vector was acting in the negative z-axis direction instead of the negative y-axis direction. This was necessary based on the coordinate system I chose to draw the triangle weir in.

Next, the geometry and initial condition files were modified as described below. Note that the files decomposePar, meshQualityDict, surfaceFeatureExtractDict, and snappyHexMeshDict were added to the system directory of the tutorial. Also, the headers and all comments were omitted for each file in this post to save space, but they are included in the attached case files. Additionally, the domain was resized to be 2.0 m long (x-direction), 1.0 m wide (y-direction), and 1.0 m tall (z-direction) with the weir (25 mm thick in x-dir., 1.0 m wide in y-dir., 0.5 m tall in z-dir. with a 90 degree triangle that had its bottom 0.25 m above the bottom of the channel) placed in the middle of the channel.

In the system directory, the following files were modified or added:

blockMeshDict:
Code:
convertToMeters 1;

xI -1;
xJ 1;
yI -0.5;
yJ 0.5;
zI 0.0;
zJ 1.0;

vertices
(
    ($xI $yI $zI)
        ($xJ $yI $zI)
        ($xJ $yJ $zI)
        ($xI $yJ $zI)
        ($xI $yI $zJ)
        ($xJ $yI $zJ)
        ($xJ $yJ $zJ)
        ($xI $yJ $zJ)
);

blocks         
(
    hex (0 1 2 3 4 5 6 7)  (100 50 50)  simpleGrading (1 1 1)
);

edges         
(
);

patches
(
        patch inlet
        (
                (0 4 7 3)
        )
        patch outlet
        (
                (1 2 6 5)
        )
        wall bottom
        (
                (0 3 2 1)
        )
        wall right
        (
                (0 1 5 4)
        )
        wall left
        (
                (3 7 6 2)
        )
        patch atmosphere
        (
                (4 5 6 7)
        )
);

mergePatchPairs
(
);
setFieldsDict:
Code:
defaultFieldValues
(
    volScalarFieldValue alpha.water 0
);

regions
(
    boxToCell
    {
        box (-1 -0.5 0) (0 0.5 0.2);

        fieldValues
        (
            volScalarFieldValue alpha.water 1
        );
    }
);
snappyHexMeshDict:
Code:
// Which of the steps to run
castellatedMesh true;
snap            true;
addLayers      false;

geometry
{
        TriangleWeir
        {
                type triSurfaceMesh;
                file "TriangleWeir.stl";
        }
};

castellatedMeshControls
{
    maxLocalCells 10000000;

    maxGlobalCells 200000000;

    minRefinementCells 0;

    nCellsBetweenLevels 3;

    features
    (
    );


    refinementSurfaces
    {
                TriangleWeir
        {
            level    (2  2);
            patchInfo
            {
                type wall;
            }
        }
    }

    // Resolve sharp angles
    resolveFeatureAngle 30;

    refinementRegions
    {
    }

    locationInMesh (0.314159 0.314159 0.314159);

    allowFreeStandingZoneFaces true;
}
   
snapControls
{
    nSmoothPatch 10; // or 15;
       
    tolerance 4.0;  // or 0.1;
   
    nSolveIter 30;

    nRelaxIter 10;

        nFeatureSnapIter 20;

        implicitFeatureSnap false;

        explicitFeatureSnap true;

        multiRegionFeatureSnap false;
}

addLayersControls
{
    relativeSizes true;

    layers
    {
        suplat
        {
            nSurfaceLayers 2;
        }
    }

    expansionRatio 1.0;

    finalLayerThickness 0.3;

    minThickness 0.1;

    nGrow 0;

    featureAngle 60;

    slipFeatureAngle 30;

    nRelaxIter 3;

    nSmoothSurfaceNormals 1;

    nSmoothNormals 3;

    nSmoothThickness 10;

    maxFaceThicknessRatio 0.5;

    maxThicknessToMedialRatio 0.3;

    minMedianAxisAngle 90;

    nBufferCellsNoExtrude 0;

    nLayerIter 50;
}

meshQualityControls
{
    #include "meshQualityDict"

    nSmoothScale 10;

    errorReduction 0.9;
}

mergeTolerance 1e-6;
meshQualityDict:
Code:
// Include defaults parameters from master dictionary
#includeEtc "caseDicts/meshQualityDict"

minFaceWeight 0.02;
surfaceFeatureExtractDict:
Code:
TriangleWeir.stl
{
    extractionMethod    extractFromSurface;

    extractFromSurfaceCoeffs
    {
        includedAngle  180;
    }

    subsetFeatures
    {
        nonManifoldEdges      no;

        openEdges      yes;
    }

        writeObj                yes;
}
decomposeParDict:
Code:
numberOfSubdomains 32;

method          scotch;

simpleCoeffs
{
    n              ( 4 2 2 );
    delta          0.001;
}

hierarchicalCoeffs
{
    n              ( 1 1 1 );
    delta          0.001;
    order          xyz;
}

metisCoeffs
{
    processorWeights ( 1 1 1 1 );
}

manualCoeffs
{
    dataFile        "";
}

distributed    no;

roots    ();
In the 0 directory, the following files were modified:

include/initialConditions:
Code:
inletFlowRate        0.02451;
pressure            0;
turbulentKE          4.14e-03;
turbulentEpsilon    4.39e-05;
Note that the above flow rate Q~(m^{3}/s) was calculated according to the equation given in the image shown below using H=0.2~m, g=9.81~m/s^{2}, and \theta=90 degrees. The coefficient C_{d} was taken to be 0.58 based on Figure 10.25 on page 599 of "Fundamentals of Fluid Mechanics, Fifth Edition" by Munson, Young, and Okiishi.

https://i.imgur.com/K2G3JAw.jpg

alpha.water:
Code:
#include        "include/initialConditions"

dimensions      [0 0 0 0 0 0 0];

internalField  uniform 0;

boundaryField
{
    inlet
    {
        type            variableHeightFlowRate;
        lowerBound      0;
        upperBound      1;
        value          uniform 0;
    }

    outlet
    {
        type            zeroGradient;
    }

    bottom
    {
        type            zeroGradient;
    }
       
        left
        {
        type            zeroGradient;
    }
       
        right
        {
        type            zeroGradient;
    }

    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value          uniform 0;
    }
       
        TriangleWeir
    {
        type            zeroGradient;
    }

    defaultFaces
    {
        type            empty;
    }
}
epsilon:
Code:
#include        "include/initialConditions"

dimensions      [0 2 -3 0 0 0 0];

internalField  uniform $turbulentEpsilon;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value          $internalField;
    }

    outlet
    {
        type                        zeroGradient;
                //type            inletOutlet;
        //inletValue      $internalField;
        //value          $internalField;
    }

    bottom
    {
        type            epsilonWallFunction;
        value          $internalField;
    }
       
        left
    {
        type            epsilonWallFunction;
        value          $internalField;
    }
       
        right
    {
        type            epsilonWallFunction;
        value          $internalField;
    }

    atmosphere
    {
        type            inletOutlet;
        inletValue      $internalField;
        value          $internalField;
    }
       
        TriangleWeir
    {
        type            epsilonWallFunction;
        value          $internalField;
    }

    defaultFaces
    {
        type            empty;
    }
}
k:
Code:
#include        "include/initialConditions"

dimensions      [0 2 -2 0 0 0 0];

internalField  uniform $turbulentKE;

boundaryField
{
    inlet
    {
        type            fixedValue;
        value          $internalField;
    }

    outlet
    {
                type                        zeroGradient;
        //type            inletOutlet;
        //inletValue      $internalField;
        //value          $internalField;
    }

    bottom
    {
        type            kqRWallFunction;
        value          $internalField;
    }
       
        left
        {
        type            kqRWallFunction;
        value          $internalField;
    }
       
        right
        {
        type            kqRWallFunction;
        value          $internalField;
    }

    atmosphere
    {
        type            inletOutlet;
        inletValue      $internalField;
        value          $internalField;
    }
       
        TriangleWeir
    {
        type            kqRWallFunction;
        value          $internalField;
    }

    defaultFaces
    {
        type            empty;
    }
}
nut:
Code:
dimensions      [0 2 -1 0 0 0 0];

internalField  uniform 0;

boundaryField
{
    inlet
    {
        type            calculated;
        value          uniform 0;
    }
       
    outlet
    {
        type            calculated;
        value          uniform 0;
    }
       
    bottom
    {
        type            nutkWallFunction;
        value          uniform 0;
    }
       
        left
        {
        type            nutkWallFunction;
        value          uniform 0;
    }
       
        right
        {
        type            nutkWallFunction;
        value          uniform 0;
    }
       
    atmosphere
    {
        type            calculated;
        value          uniform 0;
    }
       
        TriangleWeir
    {
        type            nutkWallFunction;
        value          uniform 0;
    }
       
    defaultFaces
    {
        type            empty;
    }
}
p_rgh:
Code:
#include        "include/initialConditions"

dimensions      [1 -1 -2 0 0 0 0];

internalField  uniform $pressure;

boundaryField
{
    inlet
    {
        type            zeroGradient;
    }

    outlet
    {
                type            fixedValue;
        value          uniform 0;
        //type            zeroGradient;
    }

    bottom
    {
        type            fixedFluxPressure;
    }
       
        left
        {
        type            fixedFluxPressure;
    }
       
        right
        {
        type            fixedFluxPressure;
    }

    atmosphere
    {
        type            totalPressure;
        p0              uniform 0;
    }
       
        TriangleWeir
    {
        type            fixedFluxPressure;
    }

    defaultFaces
    {
        type            empty;
    }
}
U:
Code:
#include        "include/initialConditions"

dimensions      [0 1 -1 0 0 0 0];

internalField  uniform (0 0 0);

boundaryField
{
    inlet
    {
        type            variableHeightFlowRateInletVelocity;
        flowRate        $inletFlowRate;
        alpha          alpha.water;
        value          uniform (0 0 0);
    }

    outlet
    {
        type            zeroGradient;
    }

    bottom
    {
        type            noSlip;
    }
       
        left
        {
        type            noSlip;
    }
       
        right
        {
        type            noSlip;
    }

    atmosphere
    {
        type            pressureInletOutletVelocity;
        value          uniform (0 0 0);
    }
       
        TriangleWeir
    {
        type            noSlip;
    }

    defaultFaces
    {
        type            empty;
    }
}
After all the files were modified, the following series of commands was used to construct the case and then run it. Note that since I had access to 32 cores using two computers, I was able to execute the snappyHexMesh and interFoam commands using parallel processing. If you want to use a different amount, just change the 32s to whatever you're going to use and don't forget to also change the number in your decomposeParDict file too, or else OpenFOAM will give an error output.

Code:
rm -r 0
cp -r 0.org 0
blockMesh > log.blockMesh
surfaceFeatureExtract > log.surfFeatExt
decomposePar -copyZero > log.decompPar_sHM
mpirun -np 32 snappyHexMesh -parallel > log.sHM
reconstructParMesh -mergeTol 1e-06 -time '0.002' > log.sHMreconParMesh
reconstructPar -time '0.002' > log.reconPar_sHM
cp -r ./0.002/polyMesh/* ./constant/polyMesh
rm -r ./0.002
rm -r processor*
setFields > log.setFields
decomposePar > log.decompPar_run
mpirun -np 32 interFoam -parallel > log.interFoam 2>&1
The mesh created by snappyHexMesh is shown below. Here you can see the 2 levels of refinement with 3 cells between each level, which were specified in the snappyHexMeshDict file.

https://i.imgur.com/EKQswNi.png

Finally, a pretty result image! This image was generated for the system state at 9 seconds of simulated time (I changed the writeInterval parameter in ./system/controlDict to be 1 instead of 2). Also, the surface was shaded according to the velocity magnitude.

https://i.imgur.com/fABDVRQ.png


All times are GMT -4. The time now is 08:00.