Node147 - CFD SUPPORT

Previous: Instant convergence monitoring during Up: Test case: motorBike Next: Function probe

This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.

Aerodynamic coefficients and

Aerodynamic coefficients and can be evaluated by adding additional functions to controlDict file

Configuration file controlDict is extended:

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

application     simpleFoam;

startFrom       latestTime;

startTime       0;

stopAt          endTime;

endTime         500;

deltaT          1;

writeControl    timeStep;

writeInterval   100;

purgeWrite      0;

writeFormat     binary;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

functions
{
    #include "streamLines"
    #include "cuttingPlane"
    #include "forceCoeffs"
}



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

Object libs and includes of files streamLines and cuttingPlane can be deleted for this time. File forceCoeffs reads as follows:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  dev                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

forceCoeffs1
{
    type            forceCoeffs;

    libs            ("libforces.so");

    writeControl    timeStep;
    timeInterval    1;

    log             yes;

    patches         (motorBikeGroup);
    rho             rhoInf;      // Indicates incompressible
    rhoInf          1;           // Redundant for incompressible
    liftDir         (0 0 1);
    dragDir         (1 0 0);
    CofR            (0.72 0 0);  // Axle midpoint on ground
    pitchAxis       (0 1 0);
    magUInf         20;
    lRef            1.42;        // Wheelbase length
    Aref            0.75;        // Estimated
    /*
    binData
    {
        nBin        20;          // output data into 20 bins
        direction   (1 0 0);     // bin direction
        cumulative  yes;
    }
    */
}

forceCoeffs1 computes coefficients and in direction liftDir and dragDir, data are saved after each time step in directory postProcessing/forceCoeffs1

Easy Gnuplot script named e.g. plotCdCl displays and development:

# Gnuplot script file for plotting data from file "forceCoeffs.dat"
set title "Convergence process"
set xlabel "Iterations"
set ylabel "Aerodynamics Coefficients"
plot [ ][-0.2:0.8]\
      "postProcessing/forceCoeffs1/0/forceCoeffs.dat" using 1:3 title 'Cd', \
      "postProcessing/forceCoeffs1/0/forceCoeffs.dat" using 1:4 title 'Cl'
pause mouse

Run the script:
# gnuplot plotCdCl

Figure: OpenFOAM tutorial motor bike. and development during computation

Previous: Instant convergence monitoring during Up: Test case: motorBike Next: Function probe

OpenFOAM Training by CFD Support, CFD SUPPORT, info@cfdsupport.com +420 212 243 883 © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic

Next: Model setting without an Up: Alternative formulation Previous: Alternative formulation Contents Index

Running blockMesh

Each application has its help:
# blockMesh -help

Usage: blockMesh [OPTIONS]
options:
  -blockTopology    write block edges and centres as .obj files
  -case <dir>       specify alternate case directory, default is the cwd
  -dict <file>      specify alternative dictionary for the blockMesh description
  -noFunctionObjects
                    do not execute functionObjects
  -region <name>    specify alternative mesh region
  -srcDoc           display source code in browser
  -doc              display application documentation in browser
  -help             print the usage

Using: OpenFOAM-2.2.1 (see www.OpenFOAM.org)
Build: 2.2.1-57f3c3617a2d

Parameter -help displays options of each application
Run blockMesh application in test case directory:
# cd $FOAM_RUN/icoFoam/cavity
# blockMesh
Application checkMesh displays many important about mesh:
# checkMesh

OpenFOAM Training by CFD Support, CFD SUPPORT, info@cfdsupport.com +420 212 243 883 © CFD support, s.r.o., Sokolovská 270/201, 190 00 Praha 9, Czech Republic

Previous: Advanced parameters Up: Turbo Unwrap filter – Next: TCFD – Rescue List
_{This is an automatically generated documentation by LaTeX2HTML utility. In case of any issue, please, contact us at info@cfdsupport.com.}

Usage

The usage of the filter is similar to other filters with one small difference: Because it allows (and requires) selection of different parts of the multi-part mesh, it is necessary to load all needed parts of the mesh, not just the internal mesh. The figure

demonstrates a typical selection of OpenFOAM case mesh and patches for the Turbo Unwrap filter.

Figure: Turbo Blade Post; Selection of multiple parts of the mesh.

The filter will transform the cylinder-like mesh into a box. The meaning of its new dimensions is described in the table

. In brief it can be said that the boundary $z' \equiv \zeta = 0$ is the hub patch, the boundary $z' \equiv \zeta = 1$ is the shroud patch, the boundary $x' \equiv m = 0$ is the one of inlet and outlet interfaces that is lower on the rotation axis and the boundary $x' \equiv m = 1$ is the other one (higher on rotation axis). The boundaries on minimal and maximal $y' \equiv t$ coordinates are only artificial and were originally connected to each other. The filter transforms only the cell data, not point data, so it may be necessary to apply the filter Cell data to point data afterwards to regain access to the point fields (which are necessary for usage of e.g. the Glyph filter).

Table: Coordinates of the "unwrapped" mesh. The coordinate

is relative to the full length of the hub/shroud/streamline. The coordinate $\zeta$ is relative to the full local distance between hub and shroud.

Symbol	Mapped to	Range	Meaning
			Distance along the hub/shroud/streamline.
		$(0, 2\pi)$	Circumferential angle.
$\zeta$			Distance from the hub; the "span".

The filter passes all cell data without change except for the vector fields U and URel, which are transformed into the new coordinate system $(x', y', z') \equiv (m, t, \zeta)$ . Besides these two vector fields Turbo Unwrap also creates several additional vector fields, namely UStream and URelStream which should be used to construct streamlines in the transformed mesh and URelLIC, which should be used as an input for the Surface Line Integral Convolution (SurfaceLIC) integrator when displaying realtive velocity using SurfaceLIC representation.