[Bloerb]

I have programmed a simple mesh Motion Solver. It currently moves a patch with constant velocity "vel". I now want to extend this velocity to be a function of time. The DataEntry class seems to be the way to go. I want to supply a table with time and velocity inside my dynamicMeshDict and use those for interpolation.

My first attempt is adding

#include "DataEntry.H"

and the following entry for my dataEntry

    const DataEntry<vector> vel
    (
        motionDict_.lookup("vel")
    );

And finally changing the old vector vel to the dataEntry vel.value which should give me the interpolated value

    
forAll(patchPoints, ppI)
    {
        np[patchPoints[ppI]] += vel.value(time().value())*time().deltaTValue();
    }

Since my c++ is at best rusty I was surprised it compiled without error messages but when starting the solver i got the following message:

--> FOAM FATAL ERROR: 
Not implemented

    From function Type Foam::DataEntry<Type>::value(const scalar) const
    in file /opt/openfoam30/src/OpenFOAM/lnInclude/DataEntry.C at line 73.

FOAM aborting

Has anyone an idea on how to fix this / do this correctly?

[alexeym]

Hi,

value method is implemented only in children of DataEntry class (CSV, Constant, Table, etc.).

You can find example of usage in $FOAM_SRC/mesh/extrudeModel/radial.

[Bloerb]

Thank you for the quick reply alexeym. Because of your input I now include InterpolationTable.H instead of DataEntry.H, which then itself includes it. I also had to make minor adjustments to the rest of the code. With this i can now provide a file with tabulated values. The problem is therefore solved.

I would nevertheless like to have the flexability boundary conditions have. Like choosing between table polynom etc. Is this not possible in this scope?

[alexeym]

Well, if radial example is not quite convincing, you can take a look at $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived/uniformFixedValue boundary condition.

Since you would like user to select between CSV, Polynomial, etc. you need:

1. Include DataEntry.H
2. Declare property as autoPtr<DataEntry<vector> > vel_
3. Use DataEntry::New(...) (http://foam.sourceforge.net/docs/cpp...be2ac84884862f) to create vel_ property.

You can find example of DataEntry construction on line 87 of uniformFixedValueFvPatchField.C. And you can find variants of uniformFixedValue usage (i.e. dictionary describing DataEntry) in

$ cd $FOAM_TUTORIALS
$ grep -lr uniformFixedValue *
incompressible/pimpleDyMFoam/movingCone/0/pointMotionUx
incompressible/simpleFoam/turbineSiting/0.org/U
incompressible/simpleFoam/turbineSiting/0.org/p
lagrangian/reactingParcelFilmFoam/hotBoxes/0.org/U
multiphase/interDyMFoam/ras/damBreakWithObstacle/0.org/U
multiphase/interPhaseChangeDyMFoam/propeller/0.org/U
multiphase/potentialFreeSurfaceDyMFoam/oscillatingBox/0.org/pointDisplacement

The most informative would be multiphase/interPhaseChangeDyMFoam/propeller/0.org/U, as others use Constant variant of DataEntry. Or you can refer http://www.openfoam.org/version2.1.0...conditions.php. Or concrete classes header for dictionary syntax.