[rcastilla]

Hi, I was using funkySetFields with interFoam in OpenFoam 1.6 without problems. Now, I have upgraded to 1.7.0, and compiled the funkySetFields and it gives the error:

--> FOAM FATAL IO ERROR:
Unknown patchField type constantAlphaContactAngle for patch type wall

Valid patchField types are :

41
(
advective
buoyantPressure
calculated
cyclic
directMapped
directionMixed
empty
fan
fixedFluxPressure
fixedGradient
fixedInternalValue
fixedPressureCompressibleDensity
fixedValue
freestream
freestreamPressure
inletOutlet
inletOutletTotalTemperature
mixed
oscillatingFixedValue
outletInlet
partialSlip
processor
rotatingTotalPressure
sliced
slip
symmetryPlane
syringePressure
timeVaryingMappedFixedValue
timeVaryingMappedTotalPressure
timeVaryingTotalPressure
timeVaryingUniformFixedValue
timeVaryingUniformInletOutlet
totalPressure
totalTemperature
turbulentInlet
turbulentIntensityKineticEnergyInlet
uniformDensityHydrostaticPressure
uniformFixedValue
waveTransmissive
wedge
zeroGradient
)

related to the modification of the alpha1 file.

Any idea of wath is wrong?

Robert

[gschaider]

Originally Posted by rcastilla

Hi, I was using funkySetFields with interFoam in OpenFoam 1.6 without problems. Now, I have upgraded to 1.7.0, and compiled the funkySetFields and it gives the error:

related to the modification of the alpha1 file.

Any idea of wath is wrong?

Robert

FSF only "knows" (because it is linked against that) the boundary-conditions in libfiniteVolume.so. The BC you have is application-specific. So it is either implemented in the solver or in another library. In the first case you have bad luck and must temporarily change the BC on the patch to something from that list. In the second case (BC in a library) you can add the library to the libs-list in the controlDict. The library will then be loaded in the beginning and FSF will "know" it

Bernhard

[rcastilla]

Bernhard,

I wanted to use FSF with an interFoam simulation. So, I have put the same includes and libs in the options file in the Make folder than in the interFoam source tree, I have recompiled it, and now it works perfectly.

Thanks so much!

Robert

[gschaider]

Originally Posted by rcastilla

I wanted to use FSF with an interFoam simulation. So, I have put the same includes and libs in the options file in the Make folder than in the interFoam source tree, I have recompiled it, and now it works perfectly.

An entry of the form

libs ("libmissingLibrary1.so" "libmissingLibrary2.so");

in the controlDict of the case would have had the same effect and you would not have to recompile FSF for every other solver/case

Bernhard

[steph79]

Hi,

I've been experiencing the same error when using FSF (in 2.1.1) to initialise a domain containing a constantAlphaContactAngle patch. Does anybody know the specific libraries to include in the controlDict? I know how to work around it, but it would be preferable to have a robust solution.

Thanks.

[michielm]

I think you need this one: libtwoPhaseInterfaceProperties.so
because that is the library where constantAlphaContactAngle is build-in

[shri@]

Thank you !

I had a similar problem while implementing the 'dynamicAlphaContactAngle' for my case.
For OpenFOAM 3.0.x (with swak4Foam version 0.4.0 ) you need to add
"libtwoPhaseMixture.so" and "libtwoPhaseProperties.so" to controlDict libs section for implementing dynamic contact angle.

I am looking for a way where I can inject droplets (liquid ) in VOF setup (interFoam) after each time step.

It would be great if someone can guide me.

Thank you in advance.

Shridhar