[farshadexp]

Hi FOAMers...
I'm trying to declare a new volScalarField based on an existing volScalarField, as followong:

volScalarField rhohe
(
    IOobject
    (
        "rhohe",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    rho*thermo.he()
);

No compile error.
But during run, following error is being shown:

--> FOAM FATAL ERROR: 
cannot be called for a calculatedFvPatchField
    on patch base of field rhohe in file "/home/farshad/OpenFOAM/farshad-v1812/run/fireFoam/LES/smallPoolFire2D/0/rhohe"
    You are probably trying to solve for a field with a default boundary condition.

    From function Foam::tmp<Foam::Field<Type> > Foam::calculatedFvPatchField<Type>::gradientInternalCoeffs() const [with Type = double]
    in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.

Your helps are appreciated, in advance.

[boundary93]

I think you should do the calculaton not where you create the field but Im not sure

[farshadexp]

Thanks boundary93 for your response...
I declare that in Createfields.H and also YEEqn.H. But in both cases the result is same, runtime error.

[adhiraj]

Are you creating a field rhohe and then also trying to solve an equation for it?

If so, you will need to explicitly set boundary conditions for rhohe. As far as I recall, when you multiply two fields to produce a new field, you get "calculated" boundary conditions for the new field. Solvers don't know what to do with the "calculated" boundary condition.

Hope this helps.

[farshadexp]

Dear Adhiraj
You are right, that's the point.

But, I am trying to solve "rhohe" instead of "he" in the same manner. For "he" we need no BC, and also for rho, so why we need to specify BC for new "rhohe"??
And, what's the solution

[adhiraj]

Keep in mind that he is a 'special' variable, in that it is generated internally, and is not provided by the user. This variable also comes with special boundary conditions, and it is taken care of by the code internally.

The variable rho does not seem to be so special, and so I am not 100% sure of what is happening. I think this is what happens with rho (someone more familiar with the code can explain more? ):

If you look at the rho equation, it does not seem to directly use boundary values of rho.
So maybe that is why the function gradientInternalCoeffs is not called for rho?

[farshadexp]

Thanks for explanation Adhiraj, right!
I'm looking for a solution to declare a volSacalarField based on "he", which do not need a boundary condition, because I think it's hard to specify a BC.
What is the solution? do you have any idea?!

[adhiraj]

I guess there are two options here:

1. Implement the new variable as rhohe = rho*he. For the boundary conditions, have a look at what is done for he, and maybe you can use that as a guide. Here your goal is to come up with a boundary condition that is consistent with the corresponding temperature boundary condition.

2. Reformulate the problem so that you know what boundary conditions to use, and simply read them in during simulation. So you will need to provide a rhohe file in the initial time directory.

[farshadexp]

appreciated Adhiraj...
for the first option, declaring rhohe=rho*he leads to compile error.
Declaring in YEEqn.H:

YEEqn.H:58:32: error: invalid user-defined conversion from ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >’ to ‘Foam::volScalarField& {aka Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&}’ [-fpermissive]
     volScalarField& rhohe = rho*he;

Declaring in createFields.H:

createFields.H:177:29: error: conversion from ‘const Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>’ to ‘Foam::volScalarField& {aka Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&}’ discards qualifiers [-fpermissive]
 volScalarField& rhohe = rho*he;

[adhiraj]

Sorry if my last reply was not clear, my bad

When I wrote

Implement the new variable as rhohe = rho*he.

I did not mean that the line should be directly used in code, since that would not work. I was suggesting a thought process. You will need to figure out how to implement that thought into meaningful code. Unfortunately I have not studied the code part where he is defined and boundaries set, so I cannot help you with the implementation.

[The Mad Scientist]

Farshad,

In case you have some simple boundary condition then you can use this format but this only works very few boundary types.


Info<< "Reading field h\n" << endl;
volScalarField h
(
IOobject
(
"h",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
Cp*T + fl*L,
T.boundaryField().types(),
fl.boundaryField().types()
);


If this doesn't help then you can either define your field in normal ways and calculate your boundary values somewhere in the solver.


or you can predefine your varible in you 0 directory then modify the internal field in the code given you have simple BC.

[farshadexp]

Hi Adhiraj
that was my fault. thanks for your guidance. I will try and hopefully find a solution...

Originally Posted by adhiraj

Sorry if my last reply was not clear, my bad

When I wrote



I did not mean that the line should be directly used in code, since that would not work. I was suggesting a thought process. You will need to figure out how to implement that thought into meaningful code. Unfortunately I have not studied the code part where he is defined and boundaries set, so I cannot help you with the implementation.

[farshadexp]

Hi Scientist
Based on your explanations, I will define variable. It need some manipilations (I guess). I will tell you the results.

Originally Posted by The Mad Scientist

Farshad,

In case you have some simple boundary condition then you can use this format but this only works very few boundary types.


Info<< "Reading field h\n" << endl;
volScalarField h
(
IOobject
(
"h",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
Cp*T + fl*L,
T.boundaryField().types(),
fl.boundaryField().types()
);


If this doesn't help then you can either define your field in normal ways and calculate your boundary values somewhere in the solver.


or you can predefine your varible in you 0 directory then modify the internal field in the code given you have simple BC.

[farshadexp]

Originally Posted by The Mad Scientist

Farshad,

In case you have some simple boundary condition then you can use this format but this only works very few boundary types.


Info<< "Reading field h\n" << endl;
volScalarField h
(
IOobject
(
"h",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
Cp*T + fl*L,
T.boundaryField().types(),
fl.boundaryField().types()
);


If this doesn't help then you can either define your field in normal ways and calculate your boundary values somewhere in the solver.


or you can predefine your varible in you 0 directory then modify the internal field in the code given you have simple BC.

Hi,
I tried your solution and declared a field as followings:

volScalarField rhohe
(
    IOobject
    (
        "rhohe",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ, //NO_READ,
        IOobject::AUTO_WRITE
    ),
    rho*he,
    rho.boundaryField().types(),
    he.boundaryField().types()
);

moreover, after encountering the same problem, I define a "rhohe" file based on "T" in "0" folder (obviously it's not a correct BC but I do this to check the response of the solver):

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      rhohe;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [2 -1 -2 0 0 0 0];

internalField   uniform 300;

boundaryField
{
    "(outlet|sides)"
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }

    base
    {
        type            zeroGradient; //calculated;
        //value           $internalField;
    }

    inlet
    {
        type            fixedValue;
        value           uniform 300;
    }

    frontAndBack
    {
        type            empty;
    }
}

But again, nothing is changed.

--> FOAM FATAL ERROR: 
cannot be called for a calculatedFvPatchField
    on patch base of field rhohe in file "/home/farshad/OpenFOAM/farshad-v1812/run/fireFoam/LES/smallPoolFire2D/0.00144928/rhohe"
    You are probably trying to solve for a field with a default boundary condition.

    From function Foam::tmp<Foam::Field<Type> > Foam::calculatedFvPatchField<Type>::gradientInternalCoeffs() const [with Type = double]
    in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.

[Daniel_Khazaei]

try this:

1- Declare your variable to be read from 0 directory:

volScalarField rhohe
(
    IOobject
    (
        "rhohe",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

2- Then update it somewhere in your code before solving for it:

rhohe = rho * he;
rhohe.correctBoundaryConditions();

Note: with this method you have to set correct boundary conditions for rhohe in 0 directory.