[alexio97]

Hello openfoamers. I have a problem dealing with the dimension

thermalPhaseChangeModel
(
name,
thermalPhaseChangeProperties,
twoPhaseProperties,
T,
alpha1
),
Q_pc_
(
IOobject
(
"PhaseChangeHeat",
T_.time().timeName(),
T.mesh(),
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
T.mesh(),
dimensionedScalar( "dummy", dimensionSet(1,-1,-3,0,0,0,0), 0 )
)
{

// reading rl and rv
thermalPhaseChangeProperties_.lookup("rl") >> rl;
thermalPhaseChangeProperties_.lookup("rv") >> rv;

correct();
}


// * * * * * * * * * * * * * * Member Functions * * * * * * * * * * * * * * //

void Foam::thermalPhaseChangeModels::EmpiricalRateParam eter::calcQ_pc()
{
const dimensionedScalar& rhol = twoPhaseProperties_.rho1();
const dimensionedScalar& rhov = twoPhaseProperties_.rho2();

forAll(alpha1_, cellI)
{
if (alpha1_[cellI] < 0.9 && alpha1_[cellI] > 0.01)
{
Q_pc_[cellI] = pos(T_[cellI] - T_sat_)*h_lv_*rl*alpha1_[cellI]*rhol*((T_[cellI] - T_sat_)/T_sat_) + neg(T_[cellI] -T_sat_)*h_lv_*rv*(1.0 - alpha1_[cellI])*rhov*((T_[cellI] - T_sat_)/T_sat_);


}

else
{
Q_pc_[cellI] = 0;
}
}

}

This is my code. The wmake works but when i run this solver, openfoam 2.4.0 thinks Q_pc_ as zero dimension. But as you can see, I made Q_pc_ to be (1,-1,-3,0,0,0,0). How can i solve this problem?


p.s error occurs like this
error: cannot convert ‘Foam::dimensioned<double>’ to ‘double’ in assignment
Q_pc_[cellI] = pos(T_[cellI] - T_sat_)*h_lv_*rl*alpha1_[cellI]*rhol*((T_[cellI] - T_sat_)/T_sat_) + neg(T_[cellI] -T_sat_)*h_lv_*rv*(1.0 - alpha1_[cellI])*rhov*((T_[cellI] - T_sat_)/T_sat_);

this error come when i run the program.
--> FOAM FATAL ERROR:
Different dimensions for =
dimensions : [1 -1 -3 0 0 0 0] = [0 0 0 0 0 0 0]

[olesen]

If you use something like Q_pc[index], you are already bypassing dimension checks. Your dimensions are coming from somewhere else like rhol. Might want to use the .value() method there.

[alexio97]

Originally Posted by olesen

If you use something like Q_pc[index], you are already bypassing dimension checks. Your dimensions are coming from somewhere else like rhol. Might want to use the .value() method there.

Thank you for your reply You mean q_pc already has its dimension?
Then I have to make a code something like
(pos(T_[cellI] - T_sat_)*h_lv_*rl*alpha1_[cellI]*rhol*((T_[cellI] - T_sat_)/T_sat_) + neg(T_[cellI] -T_sat_)*h_lv_*rv*(1.0 - alpha1_[cellI])*rhov*((T_[cellI] - T_sat_)/T_sat_)).value() ??

[olesen]

Originally Posted by alexio97

Thank you for your reply You mean q_pc already has its dimension?
Then I have to make a code something like
(pos(T_[cellI] - T_sat_)*h_lv_*rl*alpha1_[cellI]*rhol*((T_[cellI] - T_sat_)/T_sat_) + neg(T_[cellI] -T_sat_)*h_lv_*rv*(1.0 - alpha1_[cellI])*rhov*((T_[cellI] - T_sat_)/T_sat_)).value() ??

It looks like your Q_pc is a volScalarField - when thinking of the rest, it would pay to take a look at some of the tutorial files (the various 0/ fields) to see what how they are structured. The volScalarField has the same things: dimensions, an internal field and the boundary patches. Within OpenFOAM, you usually work on the highest level, for example adding or multiplying these volume fields. The dimension checks are done once at the top level. At the lower-level of looping, you just have an "internal" field of values, eg a scalar for each cell. These don't have any dimensions, and you wouldn't really want to have dimension checking in the inner loop. So when you are referencing an internal value like Q_pc[cellId] you are just getting the scalar value. If you start to multiply these with things that _are_ dimensioned, such as a dimensionedScalar, things get a bit weird since the plain scalar doesn't have dimension. At that stage you would normally use the .value() on the dimensionedScalar to get its plain value.


Have a play around, and you'll get the idea. Not really easy to explain at a distance.

[alexio97]

Originally Posted by olesen

It looks like your Q_pc is a volScalarField - when thinking of the rest, it would pay to take a look at some of the tutorial files (the various 0/ fields) to see what how they are structured. The volScalarField has the same things: dimensions, an internal field and the boundary patches. Within OpenFOAM, you usually work on the highest level, for example adding or multiplying these volume fields. The dimension checks are done once at the top level. At the lower-level of looping, you just have an "internal" field of values, eg a scalar for each cell. These don't have any dimensions, and you wouldn't really want to have dimension checking in the inner loop. So when you are referencing an internal value like Q_pc[cellId] you are just getting the scalar value. If you start to multiply these with things that _are_ dimensioned, such as a dimensionedScalar, things get a bit weird since the plain scalar doesn't have dimension. At that stage you would normally use the .value() on the dimensionedScalar to get its plain value.


Have a play around, and you'll get the idea. Not really easy to explain at a distance.

Thank you for your kind reply. It was very helpful! The solver perfectly works right now.

Sincerely
John