[avd28]

Hi all,

I have a custom boundary condition which defines my mesh motion. The B.C has been compiled without any errors and I have included the .so file in my controlDict. Howerver, the solver (pimpleDyMFoam) still refuses to recognize it as a valid patch-field type. Attached below is the dropbox link to my case, and custom BCs which also contains a log file with the error.

I have been through the standard openfoam discussions on this subject, but none of the suggestions there seem to work.

https://www.dropbox.com/s/ox3nefq8wj...roovy.zip?dl=0
https://www.dropbox.com/s/wygbbb0jjy...Filed.zip?dl=0

[ssss]

You have to link your library in your controlDict

libs("mylib.so");

[avd28]

As I mentioned in my original post, I have done so.

[ssss]

Sorry didn't read correctly your post. Are you sure that the .so file appears in your $FOAM_USER_LIBBIN or $FOAM_LIBBIN directories?

[avd28]

Yes, it appears in the $FOAM_USER_LIBBIN. I have confirmed it multiple times. Could you try compiling the BC and running it?

[Phil_]

Did you search & replace all the old BC-names with the new ones in the source files?

Better check all the steps given in the following post: http://www.cfd-online.com/Forums/ope...tml#post245761

Good luck

[ssss]

As I can see you are using in your pointMotionU file:

type            myRelativeVelocityPointPatchVectorField;

But in your myRelativeVelocityPointPatchVectorField.H file you are defining:

 TypeName("myRelativeVelocity");

So you should use in your pointMotionU file:

type            myRelativeVelocity;

[avd28]

Hi ssss,

Thanks, a lot. It has apparently compiled and now runs correctly, but a new error crops up.

--> FOAM FATAL IO ERROR:
Essential entry 'value' missing

file: /home/avd28/OpenFOAM/avd28-2.3.0/snz/snz1_groovy/0/pointMotionU.boundaryField.inlet from line 25 to line 29.

From function pointPatchField<Type>:ointPatchField(const fvPatch& p,const DimensionedField<Type, pointMesh>& iF,const dictionary& dict,const bool valueRequired)
in file /home/avd28/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/valuePointPatchField.C at line 96.

FOAM exiting

It would appear that this boundary condition requires, an additional entry "value" to run. Analysis of the constructors tells me that this BC requires the following entries

fixedValuePointPatchField<vector>(p, iF),
amplitude_(0.0),
refPoint_(vector::zero),
period_(0.0),
t0_(0.0)

Given my recent entry into OpenFOAM, i believed that the,

fixedValuePointPatchField<vector>(p, iF),

stood for the following line in the pointMotionU file

type myRelativeVelocity;

It now appears I was wrong. But then, what is the "value" that I'm missing here?

[ssss]

The value token needs to be set for every boundary condition, so don't worry, it wont be used in your custom BC. Just set value uniform 0 or whichever value you prefer

[avd28]

SSSS,

Whoever you are, I wish to thank you from the bottom of my heart. You've just cleared a month of logjammed work for me. Everything works as advertised. I guess I have to brush up my advanced C++ knowledge.