[s.amirzadeh]

Hi there,

I am trying to give to my inlet boundary condition a direction so I am using pressureDirectedInletOutletVelocity boundary condition. below is my Bc:

inlet
{
type pressureDirectedInletOutletVelocity;
phi phi;
rho rho;
inletDirection uniform (1 0 0);
value uniform 0;
}


I get error below when I use decomposePar or simpleFoam commands:

--> FOAM FATAL IO ERROR:
Expected a '(' while reading VectorSpace<Form, Cmpt, Ncmpts>, found on line 28 the label 0

file: /home/saeidlab/OFOAMtest(1)/airFoil2D/0/U/boundaryField/inlet/value at line 28.

From function Foam::Istream& Foam::Istream::readBegin(const char*)
in file db/IOstreams/IOstreams/Istream.C at line 92.

FOAM exiting

I do not know why it is looking for a '(', since valuse must be a scalar. even if I define it as a vector it gives the error that says value must be scalar.
Can anyone help me with this issue?

I am using openfoam10 for my simulation.

Thanks in advance

[Alczem]

Hey


For a vector such as U, you need to give 3 components to the value entry. So just change:


value uniform 0;


to


value uniform (0 0 0);


Cheers!

[s.amirzadeh]

Thank you very much, But how does that work if we define direction and velocity both in vector form? shouldn't it be a scalar representing the velocity magnitude and a vector representing direction?

[Tobermory]

Reading the BC description, I think that the "value" value is not needed, but must still be included in the boundary definition (probably because this is a derived class).

To confirm this take a look at the updateCoeffs function:

 
void Foam::pressureDirectedInletOutletVelocityFvPatchVectorField::updateCoeffs()
 {
     if (updated())
     {
         return;
     }
 
     const surfaceScalarField& phi =
         db().lookupObject<surfaceScalarField>(phiName_);
 
     const fvsPatchField<scalar>& phip =
         patch().patchField<surfaceScalarField, scalar>(phi);
 
     tmp<vectorField> n = patch().nf();
     tmp<scalarField> ndmagS = (n & inletDir_)*patch().magSf();
 
     if (phi.dimensions() == dimVelocity*dimArea)
     {
         refValue() = inletDir_*phip/ndmagS;
     }
     else if (phi.dimensions() == dimDensity*dimVelocity*dimArea)
     {
         const fvPatchField<scalar>& rhop =
             patch().lookupPatchField<volScalarField, scalar>(rhoName_);
 
         refValue() = inletDir_*phip/(rhop*ndmagS);
     }
     else
     {
         FatalErrorInFunction
             << "dimensions of phi are not correct"
             << "\n    on patch " << this->patch().name()
             << " of field " << this->internalField().name()
             << " in file " << this->internalField().objectPath()
             << exit(FatalError);
     }
 
     valueFraction() = 1.0 - pos0(phip);
 
     mixedFvPatchVectorField::updateCoeffs();
 }

... and note that the value is not used anywhere in updating the boundary values; instead it is calculated from the flux and direction.

So just set to (0 0 0) as Alczem suggests and carry on.

[Alczem]

I think the value key is, for a lot of conditions, either a placeholder or just an initial value, and then the solver computes the adequate value. So the magnitude should be taken into account if you decide to use it as an initial guess for your velocity at the boundary (for instance, value uniform (0 2 0) will tell the solver to assume a 2 m/s velocity in the Y direction for the first iteration).


I hope its clear

[Sakun]

Hi,

Sorry for the intrusion.

I am using "pressureDirectedInletOutletVelocity" as well and i would like to clear about "inletDirection".

/*--------------------------------*- C++ -*----------------------------------* \
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2112 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 1 -1 0 0 0 0];

internalField uniform (0 0 0);

boundaryField
{
INLET
{
type pressureDirectedInletOutletVelocity;
phi phi;
rho rho;
inletDirection uniform (0.63162 -0.77527 0);
value uniform (0 0 0);

}

OUTLET
{

type pressureInletOutletVelocity;
phi phi;
tangentialVelocity uniform (0 0 0);
value uniform (0 0 0);

}

CASCADE
{
type noSlip;
}

"(TOP|BOTTOM)"
{
type cyclicAMI;
}

frontAndBackPlanes
{
type empty;
}


}


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

My simulation has an inlet angle of 50.83 degrees(turbomachinery). So does it means i can define an angle in degrees in the "inletDirection" ? or do i have define as velocity component ? in this case x dir; 0.63162 y dir; -0.77527 z dir; 0