Skip to content
Permalink
Branch: master
Find file Copy path
Find file Copy path
0 contributors

Users who have contributed to this file

200 lines (143 sloc) 5.17 KB
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | Copyright (C) 2011-2016 OpenFOAM Foundation
\\/ M anipulation |
-------------------------------------------------------------------------------
License
This file is part of OpenFOAM.
OpenFOAM is free software: you can redistribute it and/or modify it
under the terms of the GNU General Public License as published by
the Free Software Foundation, either version 3 of the License, or
(at your option) any later version.
OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
FITNESS FOR A PARTICULAR PURPOSE. See the GNU General Public License
for more details.
You should have received a copy of the GNU General Public License
along with OpenFOAM. If not, see <http://www.gnu.org/licenses/>.
Class
Foam::functionObjects::forceCoeffs
Group
grpForcesFunctionObjects
Description
This function object extends the Foam::forces function object by providing
lift, drag and moment coefficients. The data can optionally be output into
bins, defined in a given direction.
Example of function object specification:
\verbatim
forceCoeffs1
{
type forceCoeffs;
libs ("libforces.so");
...
log yes;
patches (walls);
liftDir (0 1 0);
dragDir (-1 0 0);
pitchAxis (0 0 1);
magUInf 100;
lRef 3.5;
Aref 2.2;
binData
{
nBin 20;
direction (1 0 0);
cumulative yes;
}
}
\endverbatim
Usage
\table
Property | Description | Required | Default value
type | type name: forces | yes |
log | write force data to standard output | no | no
patches | patches included in the forces calculation | yes |
liftDir | lift direction | yes |
dragDir | drag direction | yes |
pitchAxis | picth axis | yes |
magUInf | free stream velocity magnitude | yes |
lRef | reference length scale for moment calculations | yes |
Aref | reference area | yes |
\endtable
Bin data is optional, but if the dictionary is present, the entries must
be defined according o
\table
nBin | number of data bins | yes |
direction | direction along which bins are defined | yes |
cumulative | bin data accumulated with incresing distance | yes |
\endtable
See also
Foam::functionObject
Foam::functionObjects::timeControl
Foam::functionObjects::forces
SourceFiles
forceCoeffs.C
\*---------------------------------------------------------------------------*/
#ifndef functionObjects_forceCoeffs_H
#define functionObjects_forceCoeffs_H
#include "forces.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
namespace functionObjects
{
/*---------------------------------------------------------------------------*\
Class forceCoeffs Declaration
\*---------------------------------------------------------------------------*/
class forceCoeffs
:
public forces
{
// Private data
// Force coefficient geometry
//- Lift
vector liftDir_;
//- Drag
vector dragDir_;
//- Pitch
vector pitchAxis_;
// Free-stream conditions
//- Velocity magnitude
scalar magUInf_;
// Reference scales
//- Length
scalar lRef_;
//- Area
scalar Aref_;
// Private Member Functions
//- Disallow default bitwise copy construct
forceCoeffs(const forceCoeffs&);
//- Disallow default bitwise assignment
void operator=(const forceCoeffs&);
protected:
//- Output file header information
virtual void writeFileHeader(const label i);
public:
//- Runtime type information
TypeName("forceCoeffs");
// Constructors
//- Construct from Time and dictionary
forceCoeffs
(
const word& name,
const Time& runTime,
const dictionary&
);
//- Destructor
virtual ~forceCoeffs();
// Member Functions
//- Read the forces data
virtual bool read(const dictionary&);
//- Execute, currently does nothing
virtual bool execute();
//- Write the forces
virtual bool write();
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace functionObjects
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //
You can’t perform that action at this time.