[bigphil]

Originally Posted by ancolli

I have the following error when i try to compile the code for a scalar T:

DCP.C: In function ‘int main(int, char**)’:
DCP.C:75:66: error: no match for ‘operator[]’ (operand types are ‘Foam::tmp<Foam::Field<double> >’ and ‘Foam::label {aka int}’)
newPatchValues[i] = -T.boundaryField()[patchID].snGrad()[i];
^
make: *** [Make/linux64GccDPOpt/DCP.o] Error 1


any idea?

fvPatchField::snGrad() return a tmp copy of a scalarField (see OpenFOAM C++ doxygen documentation); so to get your code to compile, change this line:

      newPatchValues[i] = -T.boundaryField()[patchID].snGrad()[i];

to this:

      newPatchValues[i] = -T.boundaryField()[patchID].snGrad()()[i];

However, I suggest that you store this snGrad field before you loop over each face, so as the entire patch snGrad would not be re-calculated for every faces, e.g. something like:

const scalarField patchTSnGrad = T.boundaryField()[patchID].snGrad();
forAll(newPatchValues, i)
{
      newPatchValues[i] = -patchTSnGrad[i];
}

Philip

[ancolli]

Thank you very much. I have some more questions.

1) If I need to perform mathematical operations (like log, exp, etc) to calculate new T from grad and old T. I have errors because of the different kind of variables. How can i solve it?

2) wich solver I have to select in order to verify the convergence of the BC?. Or the only change is modifying while (simple.correct Non Orthogonal())?

[bigphil]

Originally Posted by ancolli

Thank you very much. I have some more questions.

1) If I need to perform mathematical operations (like log, exp, etc) to calculate new T from grad and old T. I have errors because of the different kind of variables. How can i solve it?

If you give the mathematics here that you are trying to implement and also your initial non-compiling implementation, then I can give you pointers on the implementation.

Originally Posted by ancolli

2) wich solver I have to select in order to verify the convergence of the BC?. Or the only change is modifying while (simple.correct Non Orthogonal())?

I'm not sure I understand your question; typically for verification, you find some benchmark (analytical or numerical) and compare your results.

Philip

[ancolli]

Originally Posted by bigphil

If you give the mathematics here that you are trying to implement and also your initial non-compiling implementation, then I can give you pointers on the implementation.

could you please post some tutorials or web page?

Originally Posted by bigphil

I'm not sure I understand your question; typically for verification, you find some benchmark (analytical or numerical) and compare your results.

Philip

I am learning from laplacianFoam in steady state (the easy way). My question it is not referred to verification, instead I want to know an easy way to control convergence when BC change after each iteration. In laplacianFoam, the new nonlinear BC iterate only a number of times given by: simple.correct Non Orthogonal() setting in fvSolution

[meth]

hi Pillip,

Your posts on updating boundary condition on each iteration was very helpful to me. I am implementing a new solver using the icoFoam solver to handle the fluid-solid interaction (Vortex induced vibration). The vibration of the solid is taken into the account by assuming the fluid is in a non-inertial frame vibrate on opposite to the solid motion while the solid stay still. The solid motion due to the fluid forces are solve inside the solver and update the boundary condition accordingly in each iteration.

My question:

Since fluid is in a non-inertial frame the acceleration of the frame needs to add into the navier stokes equations. For that I defined a field variable ddy. This accelaration is a uniform value across the fluid. I can update the boundary condition as you said. Can you please tell me how to update the internal field as well? I have defined the internal field initially as a uniform value.

Many thanks,

Methma

[suman91]

Hi,

This is an old thread but am trying to do the same thing, so posting my doubt here.

I am using OpenFOAM 2.4.0 and using pisoFoam solver. I want to change the fixedGradient B.C at each time loop. So I followed what was suggested here:

fixedGradientFvPatchVectorField& wallPatch = refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchID]);

wallPatch.gradient() = dU_dy;

dU_dy is some "double" variable for which I calculate something.

But I get this error:
"fixedGradientFvPatchVectorField’ was not declared in this scope"

Please suggest where am I going wrong. Thank you.

[gschaider]

Originally Posted by suman91

Hi,

This is an old thread but am trying to do the same thing, so posting my doubt here.

I am using OpenFOAM 2.4.0 and using pisoFoam solver. I want to change the fixedGradient B.C at each time loop. So I followed what was suggested here:

fixedGradientFvPatchVectorField& wallPatch = refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchID]);

wallPatch.gradient() = dU_dy;

dU_dy is some "double" variable for which I calculate something.

But I get this error:
"fixedGradientFvPatchVectorField’ was not declared in this scope"

Please suggest where am I going wrong. Thank you.

That's the technical wonder of Polymorphism at work: your source doesn't know the class but the executable does. Try including fixedGradientFvPatchFields.H

[suman91]

Hi Bernhard,

I have in included in myfile:

#include "fixedGradientFvPatchField.H"

Still am gettinhe the error. Just for your reference an pasting the start part of my file here. insertModification.H is where I am trying my thing.

#include "fvCFD.H"
#include "singlePhaseTransportModel.H"
#include "turbulenceModel.H"
#include "fixedGradientFvPatchField.H"

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

int main(int argc, char *argv[])
{
    #include "setRootCase.H"

    #include "createTime.H"
    #include "createMesh.H"
    #include "createFields.H"
    #include "initContinuityErrs.H"

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

    Info<< "\nStarting time loop\n" << endl;

    while (runTime.loop())
    {
        Info<< "Time = " << runTime.timeName() << nl << endl;

        #include "readPISOControls.H"
        #include "CourantNo.H"

    #include "insertModification.H"

        // Pressure-velocity PISO corrector
        {
            // Momentum predictor

            fvVectorMatrix UEqn
            (
                fvm::ddt(U)
              + fvm::div(phi, U)
              + turbulence->divDevReff(U)
            );

[gschaider]

Originally Posted by suman91

Hi Bernhard,

I have in included in myfile:

#include "fixedGradientFvPatchField.H"

Still am gettinhe the error. Just for your reference an pasting the start part of my file here. insertModification.H is where I am trying my thing.

Fields.H not Field.H. The "s" is important

[bigphil]

Originally Posted by ancolli

I have the following error when i try to compile the code for a scalar T:

DCP.C: In function ‘int main(int, char**)’:
DCP.C:75:66: error: no match for ‘operator[]’ (operand types are ‘Foam::tmp<Foam::Field<double> >’ and ‘Foam::label {aka int}’)
newPatchValues[i] = -T.boundaryField()[patchID].snGrad()[i];
^
make: *** [Make/linux64GccDPOpt/DCP.o] Error 1


any idea?

Hi,

Can you post your code segment?

I think the problem is "snGrad()" returns a "tmp" of a field, so either you modify the code to be:

      newPatchValues[i] = -T.boundaryField()[patchID].snGrad()()[i];

or a better solution (no need to re-generate the entire snGrad filed every iteration) would be to store the snGrad field:

const scalarField TsnGrad= T.boundaryField()[patchID].snGrad();
forAll(newPatchValues, i)
{
      newPatchValues[i] = -TsnGrad[i];
}

Philip

[suman91]

Hi Bernhard,
It is working. Was indeed a spell typo. Thanks a lot for your help.


Hi Philip,
It seems the error was because of a typo. Here is a section of my code:

label patchID = mesh.boundaryMesh().findPatchID("channelWall");
label nFaces = mesh.boundaryMesh()[patchID].size();
for(int facei = 0 ; facei<nFaces; facei++)
{
  // doing some calculations here ....

  const fixedGradientFvPatchVectorField& wallPatch = refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchID]); 
   
 wallPatch.gradient()[facei] == vector(0, dU_dy, 0);

Hoping this will set the gradient calculated for each face on the concerned patch.
Thank you.

[suman91]

Hi,

I have a doubt related to my last post.

 const fixedGradientFvPatchVectorField& wallPatch =    refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchID]);

for(int facei = 0 ; facei<nFaces; facei++)
{
   /****  
     calculation of some gradient
   ***/  

   Info<<" Gradient of face number "<< facei << "   Before changing is  "<<endl;
   Info<<    wallPatch.gradient()[facei]<<endl;

   wallPatch.gradient()[facei] == vector(du_dy, 0, 0);

   Info<<"  After changing is  "<<endl;
   Info<<    wallPatch.gradient()[facei]<<endl;

}

Problem is when I see the values in output, both values for before and after remain same. Here is a small section of the output

Face number   0
du_dy   -0.00022415
 Gradient of face number 0   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)
Face number   1
du_dy   -0.00022415
 Gradient of face number 1   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)
Face number   2
du_dy   -0.00022415
 Gradient of face number 2   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)
Face number   3
du_dy   -0.00022415
 Gradient of face number 3   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)

Thank you in advance.

[bigphil]

Originally Posted by suman91

Hi,

I have a doubt related to my last post.

 const fixedGradientFvPatchVectorField& wallPatch =    refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchID]);

for(int facei = 0 ; facei<nFaces; facei++)
{
   /****  
     calculation of some gradient
   ***/  

   Info<<" Gradient of face number "<< facei << "   Before changing is  "<<endl;
   Info<<    wallPatch.gradient()[facei]<<endl;

   wallPatch.gradient()[facei] == vector(du_dy, 0, 0);

   Info<<"  After changing is  "<<endl;
   Info<<    wallPatch.gradient()[facei]<<endl;

}

Problem is when I see the values in output, both values for before and after remain same. Here is a small section of the output

Face number   0
du_dy   -0.00022415
 Gradient of face number 0   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)
Face number   1
du_dy   -0.00022415
 Gradient of face number 1   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)
Face number   2
du_dy   -0.00022415
 Gradient of face number 2   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)
Face number   3
du_dy   -0.00022415
 Gradient of face number 3   Before changing is  
(0 0 0)
  After changing is  
(0 0 0)

Thank you in advance.

You should not use the "==" operator; you should use the "=" operator to assign the face value.

The "==" operator is just necessary when assigning the value to an entire fixedValue-type boundary condition.

Philip

[suman91]

Hi Philip,

Thank you so much for the reply. I changed '==' to '=', then it gave me the following error:

error: passing ‘const Foam::Vector<double>’ as ‘this’ argument discards qualifiers [-fpermissive]
  wallPatch.gradient()[facei] = vector(du_dy, 0, 0);

A bit of searching and I found that declaring wallPatch as a 'const' was the problem. So I changed it to:

fixedGradientFvPatchVectorField& wallPatch = refCast<fixedGradientFvPatchVectorField>(U.boundaryField()[patchID]);

Now on printing, I see that the values are changing. Thanks a lot again for the reply.

Suman

[suman91]

Hi there,

Am having some problem in solving flow over backward facing step in OpenFOAM. I am using LES and Smagorinsky Model. At start it all goes well but after some time utau values at the wall starts increasing and the deltaT of simulation goes on decreasing (till if falls to 10^-12 or so order). I cannot detect what is the problem. I have modified the pisoFoam solver so impose stress boundary condition using the 'fixedGradient' feature of OpenFOAM.

Am attaching my required files here. Please have a look and suggest where am I going wrong. Will be waiting for a reply.

solver.tar.gz

TestCase.tar.gz

[suman91]

Hi there,

I think the problems are coming with the pressure solver settings. At t=0.01 pressure values are about -120 at the inlet and then increases linearly to close to zero at the outlet. But at T=0.05, it falls down to -4000 approx. Obviously in an incompressible flow, the absolute value of pressure does not matter, it is the gradient that matters. But what I am not understanding are such low values. Considering inlet velocity has a magnitude of 10 in the x direction (which is max amongst all 3 directions), a value of -50 to -70 may still be understandable but -4000, am not getting at all. Not understanding why the pressure field is behaving such. Maybe that is triggering the problem.

[suman91]

Hi,

Back again with an update on this same issue. So to start with, setting the gradient at the wall was not so much of a good idea it seems. Somehow the wall normal velocity was being calculated to be a non zero value at the wall. This might be one of the reasons for the solver to blow up in that manner. The modified code I am using now, uses fixedValue (0 0 0) as a boundary condition at the wall and in the modified solver, I calculate the velocity at the wall using the gradient and set the velocity. The solver now runs properly and does not blow up.

The only issue am facing with this is, the reynolds stress when calculated comes out to be very less; flow is not becoming turbulent only. Am wondering if it's an issue with the gradient schemes being used or not. If anyone has any views on this, it will be really helpful.

So the question is, what is the best gradient scheme to be used for solving incompressible turbulent flow (using LES) in openFOAM?

Sorry for maintaining two threads for the same topic. I will from now on post the updates on one particular thread itself:

Link: http://www.cfd-online.com/Forums/ope...tml#post623038

[S.Colucci]

Dear Suman,
I have a similar problem, that is my piece of code

PtrList<PtrList<volScalarField> > Index(yindex.size());

Index.set(0, new PtrList<volScalarField>(2));

Index[0].set
(
0,
new volScalarField
(
IOobject
(
"Index.pressure" ,
this->pair_.phase1().time().timeName(),
this->pair_.phase1().mesh(),
IOobject::NO_READ,
IOobject::NO_WRITE
),
Np_[0]*(p - one_p*pmin_[0])/( one_p*pmax_[0] - one_p*pmin_[0] )
)
);
// correct internalField
forAll(Index[0][0],celli)
{
Index[0][0][celli] = floor(Index[0][0][celli]);
}
// correct BC
forAll(Index[0][0].boundaryField(), patchi)
{

scalarField newPatchValues(Index[0][0].boundaryField()[patchi].size(),scalar(0));

forAll(Index[0][0].boundaryField()[patchi],i)
{
newPatchValues[i] = floor(Index[0][0].boundaryField()[patchi][i]);
}

Index[0][0].boundaryField()[patchi] == newPatchValues;
}

Commenting the last line

Index[0][0].boundaryField()[patchi] == newPatchValues

it compiles and the values stored in newPatchValues are correct, so it seems that the problem is in assigning a new bc value to Index. That is the error:

error: no match for ‘operator==’ (operand types are ‘const Foam::fvPatchField<double>’ and ‘Foam::scalarField {aka Foam::Field<double>}’)
Index[0][0].boundaryField()[patchi] == newPatchValues;

If I substitute

Index[0][0].boundaryField()[patchi] == newPatchValues

with

Index[0][0].boundaryField()[patchi] = newPatchValues

I have the following error
error: passing ‘const Foam::fvPatchField<double>’ as ‘this’ argument of ‘void Foam::fvPatchField<Type>:perator=(const Foam::UList<T>&) [with Type = double]’ discards qualifiers [-fpermissive]
Index[0][0].boundaryField()[patchi] = newPatchValues;

It seems to be the same problem as you, but I do not have any const!
Any idea?
Simone

[S.Colucci]

Originally Posted by bigphil

Yes, sorry that was a typo.

Best regards,
Philip

Dear Philip,
I post here the same problem that I posted in an other thread since here it is older but seems more appropriate

...

I have a similar problem, that is my piece of code

PtrList<PtrList<volScalarField> > Index(yindex.size());

Index.set(0, new PtrList<volScalarField>(2));

Index[0].set
(
0,
new volScalarField
(
IOobject
(
"Index.pressure" ,
this->pair_.phase1().time().timeName(),
this->pair_.phase1().mesh(),
IOobject::NO_READ,
IOobject::NO_WRITE
),
Np_[0]*(p - one_p*pmin_[0])/( one_p*pmax_[0] - one_p*pmin_[0] )
)
);
// correct internalField
forAll(Index[0][0],celli)
{
Index[0][0][celli] = floor(Index[0][0][celli]);
}
// correct BC
forAll(Index[0][0].boundaryField(), patchi)
{

scalarField newPatchValues(Index[0][0].boundaryField()[patchi].size(),scalar(0));

forAll(Index[0][0].boundaryField()[patchi],i)
{
newPatchValues[i] = floor(Index[0][0].boundaryField()[patchi][i]);
}

Index[0][0].boundaryField()[patchi] == newPatchValues;
}

Commenting the last line

Index[0][0].boundaryField()[patchi] == newPatchValues

it compiles and the values stored in newPatchValues are correct, so it seems that the problem is in assigning a new bc value to Index. That is the error:

error: no match for ‘operator==’ (operand types are ‘const Foam::fvPatchField<double>’ and ‘Foam::scalarField {aka Foam::Field<double>}’)
Index[0][0].boundaryField()[patchi] == newPatchValues;

If I substitute

Index[0][0].boundaryField()[patchi] == newPatchValues

with

Index[0][0].boundaryField()[patchi] = newPatchValues

I have the following error
error: passing ‘const Foam::fvPatchField<double>’ as ‘this’ argument of ‘void Foam::fvPatchField<Type>:perator=(const Foam::UList<T>&) [with Type = double]’ discards qualifiers [-fpermissive]
Index[0][0].boundaryField()[patchi] = newPatchValues;

It seems to be the same problem as you, but I do not have any const!
Any idea?
Simone

[bigphil]

Hi Simone,

This error:

error: passing ‘const Foam::fvPatchField<double>’ as ‘this’ argument of ‘void Foam::fvPatchField<Type>::operator=(const Foam::UList<T>&) [with Type = double]’ discards qualifiers [-fpermissive]

is saying that this 'Index[0][0].boundaryField()[patchi]' is const.

From this code:

PtrList<PtrList<volScalarField> > Index(yindex.size());

Index.set(0, new PtrList<volScalarField>(2));

Index[0].set 
(
0,
new volScalarField
(
IOobject
(
"Index.pressure" ,
this->pair_.phase1().time().timeName(),
this->pair_.phase1().mesh(),
IOobject::NO_READ,
IOobject::NO_WRITE
),
Np_[0]*(p - one_p*pmin_[0])/( one_p*pmax_[0] - one_p*pmin_[0] )
)
);
// correct internalField
forAll(Index[0][0],celli)
{
Index[0][0][celli] = floor(Index[0][0][celli]);
} 
// correct BC
forAll(Index[0][0].boundaryField(), patchi)
{

scalarField newPatchValues(Index[0][0].boundaryField()[patchi].size(),scalar(0));

forAll(Index[0][0].boundaryField()[patchi],i)
{
newPatchValues[i] = floor(Index[0][0].boundaryField()[patchi][i]);
}

Index[0][0].boundaryField()[patchi] == newPatchValues; 
}

it should not be const, and the code should compile; it compiles for me in foam-extend-32 (I would expect the same in other version too); of course I had to make some unrelated changes where I replace "yindex.size" with "1", "Np_[0]*(p - one_p*pmin_[0])/( one_p*pmax_[0] - one_p*pmin_[0] )" with "mag(U)", "this->pair_.phase1().time()" with "runTime" and "this->pair_.phase1().mesh()" with "mesh".

Are you sure this is the code you are compiling? did you, for example, post "simplified" code? If possible I would suggest making a very simple OpenFOAM utility that shows this compilation problem and then upload this for others to try.

Philip