[Kummi]

Hello Foamers,
In my work, I'm calculating pressure through the following equation,

del2(p2) = -(f1+f2*(rho*V)) * del.(rho*V) - (rho*V) . del(f1+f2*(rho*V))

My code gets compiled successfully. But, while running case file, it came up with the error,

--> FOAM FATAL ERROR:
gradientInternalCoeffs cannot be called for a calculatedFvPatchField
on patch hotSide of field sqr(p) in file "/home/kumaresh/OpenFOAM/kumaresh-2.1.1/CASE_darcyFoam/@20200110_ErgunFoam/CASE2_2D_test_1hr/0/sqr(p)"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::gradientInternalCoef fs() const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.

I have checked few other threads related to this error. Most comments are related to problem with boundary conditions. I even tried adopting different strategics for this case. But it results in same error.

• The problem is with "p2 = sqr(p)" as quoted in error.
• Under createFields:

  volScalarField p
  (
  IOobject
  (
  "p",
  runTime.timeName(),
  mesh,
  IOobject::MUST_READ,
  IOobject::AUTO_WRITE
  ),
  mesh
  );
  Info<< "Reading field square of p\n" << endl;
  volScalarField p2(sqr(p));

• Problem with defaultFvPatchField gradientInternalCoeffs - Here in the link, it was said that, "You are probably trying to solve for a field with a default boundary condition."
  This likely means that your boundary condition hasn't been linked in at all. So that my boundary condition has to be linked ?
  

**while solving the equation for only Pressure (p) variable without square term - the case gets compiled and runs good.

Anyone have some ideas as how to resolve the above error and proceed further.
Thank you

[Kummi]

I checked few threads again..
Unexplained Error - Based on the explanation in this thread, I add a new read constructor for p2 in createFields.H as,

volScalarField p2
(
IOobject
(
"p2",
runTime.timeName(),
mesh,
IOobject::MUST_READ_IF_MODIFIED,
//IOobject::NO_READ,
IOobject::AUTO_WRITE
),
//mesh
sqr(p)
//dimensionedScalar("p2", dimensionSet(2,-2,-4,0,0,0,0),0)
);

and defined p2 inside 0 boundary condition as,

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object p2;

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [ 2 -2 -4 0 0 0 0 ];
internalField uniform 101325;
boundaryField
{
hotSide
{
type calculated;
value $internalField;
}

right
{
type symmetryPlane;
}
top
{
type calculated;
value $internalField;
}

bottom
{
type zeroGradient;
}

front
{
type empty;
}

back
{
type empty;
}

Compilation - no problem
While running case file, there comes same error as:

--> FOAM FATAL ERROR:

gradientInternalCoeffs cannot be called for a calculatedFvPatchField
on patch hotSide of field p2 in file "/home/kumaresh/OpenFOAM/kumaresh-2.1.1/CASE_darcyFoam/@20200110_ErgunFoam/CASE2_2D_test_1hr/0/p2"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::gradientInternalCoef fs() const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.

FOAM exiting

Kindly someone suggest me some ideas

Thank you

[Kummi]

I feel there is problem with the declaration of code - in an implicit squared term.

del2(p2) = -(f1+f2*(rho*V)) * del.(rho*V) - (rho*V) . del(f1+f2*(rho*V))

• fvm::laplacian(p2) == - (2*T*R)*(((f1+(f2*rho*Ux))*RRg) + (rho*Uy*gradBigxx))

Such declaration is right ??
volScalarField p2(sqr(p)); //based on volScalarField p

[adhiraj]

A couple of things I notice here, which may help.

1. You have a new variable p2 which you are defining as the square of p. Doing that may not set proper boundary conditions on p2. My guess is that the boundary conditions of p2 are being set to 'calculated', and thus you cannot solve an equation for p2.

2. You provide a constructor for p2 in another attempt, but the p2 file has 'calculated' boundaries.

Since p2 is the variable you intend to use in the formulation, you need to figure out what boundary conditions make sense for it. Then initialize p2 accordingly.

See if that helps.

[Kummi]

Thank you for your response Adjiraj.
p2 (square of pressure) used in my formulation. There is no specific boundary condition for variable p2 because it is just square of pressure.
Then how to initialize p2 accordingly?
Correct me if Im wrong please

[adhiraj]

Originally Posted by Kummi

p2 (square of pressure) used in my formulation. There is no specific boundary condition for variable p2 because it is just square of pressure.

If you are solving an equation for any variable, you will almost always need to prescribe boundary conditions for it. In this case you will need to derive the boundary conditions from the corresponding boundary for p.

Originally Posted by Kummi

Then how to initialize p2 accordingly?

Once again, determine the appropriate initial conditions and boundary conditions from those of p.

Hope this helps.

[Kummi]

Dear Adhiraj,
Thank you for your comments.
As per your point, in order to solve the variable p2 in the equation, I should prescribe the appropriate initial and boundary condition for p2 based on the corresponding boundary p.

In this case you will need to derive the boundary conditions from the corresponding boundary for p.

As you mentioned, I should derive the boundary condition ?? Could you please elaborate your explanation? and if possible can you please highlight any such problems before.. Because I don't find such cases.
For pressure p, I have defined reasonable boundary conditions (below)

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object p;

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [ 1 -1 -2 0 0 0 0 ];
internalField uniform 101325;
boundaryField
{
hotSide
{
type fixedValue;
value $internalField;
}

right
{
type symmetryPlane;
}

top
{
type fixedValue;
value $internalField;
}

bottom
{
type zeroGradient;
}

front
{
type empty;
}

back
{
type empty;
}

[Kummi]

In comment 2 of this thread, p2 is fitted with *calculated* boundary condition. I dont find anyother appropriate boundary condition will fit for p2.
Kindly share some ideas. Thank you

[adhiraj]

Yes, you need to derive the boundary conditions and initial conditions for a new variable.

For example, if at a particular boundary the boundary condition for p is 'fixedValue' with a value of 10, p2 at the boundary can be 'fixedValue', with a value of . Use the same process for other boundaries and the initial condition.

The 'calculated' boundary condition is not really a true boundary condition that solvers can use. It is simply a placeholder.

[Kummi]

Dear Adhiraj,
Thank you for your comments.
As you mentioned, I defined p2 boundary with 'fixedValue'. It ends up with same error.

--> FOAM FATAL ERROR:

gradientInternalCoeffs cannot be called for a calculatedFvPatchField
on patch hotSide of field p2 in file "/home/kumaresh/OpenFOAM/kumaresh-2.1.1/CASE_darcyFoam/@20200110_ErgunFoam/CASE2_2D_test_1hr/0/p2"
You are probably trying to solve for a field with a default boundary condition.

From function calculatedFvPatchField<Type>::gradientInternalCoef fs() const
in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.

For your verification, I'm attaching the solver and case files. Kindly check it in your leisure time please. Thank you once again.

[adhiraj]

The error message seems to indicate that the code is still seeing p2 with 'calculated' boundary condition.

In your createFields.H file, why don't you initialize p2 like this?

Info<< "Reading field square of p\n" << endl;

volScalarField p2
(
    IOobject
    (
        "p2",
        runTime.timeName(),
        mesh,
        IOobject::MUST_READ,
        IOobject::AUTO_WRITE
    ),
    mesh
);

[Kummi]

Dear Adhiraj,
Thank you very much. It worked. Then, I guess - no need to solve p. I will solve p2 directly by taking the squared value.
No more errors.

[Kummi]

Dear Adhiraj,
Irrespective of this thread caption, I have one more question. In my work, I need to resolve two variables U and p.
As given in the attachment, I derived 2 equations for velocities to calculate Ux and Uy.
Followed by the pressure equation to solve pressure. Firstly, once after resolving velocities along x and y, pressure will be solved.

I defined the equations in OpenFOAM, gets compiled and the case runs without error. During post-processing, I dont find change in velocity inside my domain. However, the pressure (p2) variable is changed. Quite confused here. I guess my syntax is right.

I'm hereby attaching my code and case files.

If you are free, kindly check it please.
Thank you

[adhiraj]

Originally Posted by Kummi

Dear Adhiraj,
Thank you very much. It worked. Then, I guess - no need to solve p. I will solve p2 directly by taking the squared value.
No more errors.

It may be useful for your understanding of OpenFOAM if you can figure out why this approach works, while the other does not.

Originally Posted by Kummi

Irrespective of this thread caption, I have one more question.

Please create a new thread for the new question.

[Kummi]

Originally Posted by adhiraj

It may be useful for your understanding of OpenFOAM if you can figure out why this approach works, while the other does not.
Please create a new thread for the new question.

Understood the reason behind the approach and got your valid points.
Thank you Adhiraj for your valuable time.
*I will post my new query as a new thread.