How the boundary conditions are called in the OpenFOAM solvers?

openfoammaofnepo · February 1, 2014, 10:05

Dear All,

I was wondering how the boundary conditions subroutines are called ?

Let us take an example:

Code:

OpenFOAM/OpenFOAM-2.1.1/tutorials/compressible/rhoPimpleFoam/les/pitzDaily

In the file:

Code:

U/0

we have the following boundary conditions for the inlet:

Code:

    inlet
    {
        type            turbulentInlet;
        referenceField  uniform (10 0 0);
        fluctuationScale (0.02 0.01 0.01);
        value           uniform (10 0 0);
    }

Does anybody know in which part of the solver is calling the turbulentInlet's subroutine? I am asking this questions because I would like to implement my own BC type in openfoam.

Thank you in advance!

hjasak · February 3, 2014, 01:54

Easy:
- on correctBoundaryConditions() for a field
- on updateCoeffs() at matrix creation

correctBoundaryConditions is also called after the linear solver call automatically.

Enjoy,

Hrv

openfoammaofnepo · February 3, 2014, 12:16

Thank you so much, Hrvoje!

About the first one, I get it in the

Code:

src/OpenFOAM/fields/GeometricFields/GeometricField/GeometricField.C

I can get the following lines of codes:

Code:

// Correct the boundary conditions
template<class Type, template<class> class PatchField, class GeoMesh>
void Foam::GeometricField<Type, PatchField, GeoMesh>::
correctBoundaryConditions()
{
    this->setUpToDate();
    storeOldTimes();
    boundaryField_.evaluate();
}

Here about the function evaluation(), I cannot find where it is defined. In the following source file:

Code:

src/OpenFOAM/fields/GeometricFields/GeometricField/GeometricField.H

It is declared as

Code:

            //- Evaluate boundary conditions
            void evaluate();

But it is virtual function here. Could you please give me some hints about where it is defined assuming we are still talking about the turbulentInlet? Thank you very much.

openfoammaofnepo · February 3, 2014, 12:21

About the updateCoeffs in the turbulentInlet boundary conditions

Code:

OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/fields/fvPatchFields/derived/turbulentInlet

It has the following specific forms:

Code:

template<class Type>
void turbulentInletFvPatchField<Type>::updateCoeffs()
{
    if (this->updated())
    {
        return;
    }

    if (curTimeIndex_ != this->db().time().timeIndex())
    {
        Field<Type>& patchField = *this;

        Field<Type> randomField(this->size());

        forAll(patchField, facei)
        {
            ranGen_.randomise(randomField[facei]);
        }

        // Correction-factor to compensate for the loss of RMS fluctuation
        // due to the temporal correlation introduced by the alpha parameter.
        scalar rmsCorr = sqrt(12*(2*alpha_ - sqr(alpha_)))/alpha_;

        patchField =
            (1 - alpha_)*patchField
          + alpha_*
            (
                referenceField_
              + rmsCorr*cmptMultiply
                (
                    randomField - 0.5*pTraits<Type>::one,
                    fluctuationScale_
                )*mag(referenceField_)
            );

        curTimeIndex_ = this->db().time().timeIndex();
    }

    fixedValueFvPatchField<Type>::updateCoeffs();
}

In the above mentioned codes, the updateCoeffs() from the fixedValue boundary conditions type is used

Code:

fixedValueFvPatchField<Type>::updateCoeffs();

What is the role of this line? in the source files for fixedValue, I did not find any information about the relevant definitions there. Could anybody share some information about this problem? Thank you so much.

++++++++++++++++++++++++++++++++++++++++++++++++++ ++++++++++++++++++++++++++++++++++++++++++++++++++ ++++++++++++++++++++++++++++++++++
As a record how I understand this, I put the answer here:

evaluate() is defined in

Code:

src/OpenFOAM/fields/GeometricFields/GeometricField/GeometricBoundaryField.C

The structure is:

Code:

template<class Type, template<class> class PatchField, class GeoMesh>
void Foam::GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::
evaluate()
{
    if (debug)
    {
        Info<< "GeometricField<Type, PatchField, GeoMesh>::"
               "GeometricBoundaryField::"
               "evaluate()" << endl;
    }

    if
    (
        Pstream::defaultCommsType == Pstream::blocking
     || Pstream::defaultCommsType == Pstream::nonBlocking
    )
    {
        label nReq = Pstream::nRequests();

        forAll(*this, patchi)
        {
            this->operator[](patchi).initEvaluate(Pstream::defaultCommsType);
        }

        // Block for any outstanding requests
        if
        (
            Pstream::parRun()
         && Pstream::defaultCommsType == Pstream::nonBlocking
        )
        {
            Pstream::waitRequests(nReq);
        }

        forAll(*this, patchi)
        {
            this->operator[](patchi).evaluate(Pstream::defaultCommsType);
        }
    }
    else if (Pstream::defaultCommsType == Pstream::scheduled)
    {
        const lduSchedule& patchSchedule =
            bmesh_.mesh().globalData().patchSchedule();

        forAll(patchSchedule, patchEvali)
        {
            if (patchSchedule[patchEvali].init)
            {
                this->operator[](patchSchedule[patchEvali].patch)
                    .initEvaluate(Pstream::scheduled);
            }
            else
            {
                this->operator[](patchSchedule[patchEvali].patch)
                    .evaluate(Pstream::scheduled);
            }
        }
    }
    else
    {
        FatalErrorIn("GeometricBoundaryField::evaluate()")
            << "Unsuported communications type "
            << Pstream::commsTypeNames[Pstream::defaultCommsType]
            << exit(FatalError);
    }
}

openfoammaofnepo · February 5, 2014, 07:50

No Body also interested in this issue?

peteryuan · February 5, 2014, 10:27

As a newbie I asked a similar question in my latest post:
http://www.cfd-online.com/Forums/ope...tempratur.html

Quote:

"In externalCoupledMixedFvPatchField.C line 698 there is this evaluate() function defined. I supose that is the function at the top level and would do all the actual works for this class, like readData, writeData and so on. Now for example an object of this class is created with /0/T file and during runtime this evaluate() function is executed (I think). Could anyone tell me where is this function called during runtime? I use chtMultiRegionFoam, searched a lot in the code but still do not have a clue where this or any of the functions from that class is called. "

Here I find my key word "evaluate()":

Code:

correctBoundaryConditions() {
     this->setUpToDate();
     storeOldTimes();
     boundaryField_.evaluate(); }

I guess that all classes for BC have this .evaluate() member function... During runtime of a solver, after an object being created, the evaluate() functions are called with this correctBoundaryConditions(). Each BC class has a different .evaluate().
Am I right?

openfoammaofnepo · February 5, 2014, 18:33

Yes, I agree with you. I also did some digging into the source files. But do you know the role of the following lines:

Code:

fixedValueFvPatchField<Type>::updateCoeffs();

openfoammaofnepo · February 20, 2014, 16:46

I did not find this function in the source:

fixedValueFvPatchField.H

Sorry for my limit C++ skills. Does anybody know where I can find this function,

Code:

fixedValueFvPatchField<Type>::updateCoeffs();

?

Quote:

Originally Posted by openfoammaofnepo

Yes, I agree with you. I also did some digging into the source files. But do you know the role of the following lines:

Code:

fixedValueFvPatchField<Type>::updateCoeffs();

hjasak · February 20, 2014, 17:02

Please read up on virtual functions - this is basic C++

Hrv

openfoammaofnepo · April 10, 2014, 07:30

For my record, actually, the following lines:

Code:

fixedValueFvPatchField<Type>::updateCoeffs();

did nothing but just to set the bool variable update() to be true.

The function updateCoeffs is defined in:

Code:

fvPatchField.H

Quote:

Originally Posted by openfoammaofnepo

About the updateCoeffs in the turbulentInlet boundary conditions

Code:

OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/fields/fvPatchFields/derived/turbulentInlet

It has the following specific forms:

Code:

template<class Type>
void turbulentInletFvPatchField<Type>::updateCoeffs()
{
    if (this->updated())
    {
        return;
    }

    if (curTimeIndex_ != this->db().time().timeIndex())
    {
        Field<Type>& patchField = *this;

        Field<Type> randomField(this->size());

        forAll(patchField, facei)
        {
            ranGen_.randomise(randomField[facei]);
        }

        // Correction-factor to compensate for the loss of RMS fluctuation
        // due to the temporal correlation introduced by the alpha parameter.
        scalar rmsCorr = sqrt(12*(2*alpha_ - sqr(alpha_)))/alpha_;

        patchField =
            (1 - alpha_)*patchField
          + alpha_*
            (
                referenceField_
              + rmsCorr*cmptMultiply
                (
                    randomField - 0.5*pTraits<Type>::one,
                    fluctuationScale_
                )*mag(referenceField_)
            );

        curTimeIndex_ = this->db().time().timeIndex();
    }

    fixedValueFvPatchField<Type>::updateCoeffs();
}

In the above mentioned codes, the updateCoeffs() from the fixedValue boundary conditions type is used

Code:

fixedValueFvPatchField<Type>::updateCoeffs();

What is the role of this line? in the source files for fixedValue, I did not find any information about the relevant definitions there. Could anybody share some information about this problem? Thank you so much.

++++++++++++++++++++++++++++++++++++++++++++++++++ ++++++++++++++++++++++++++++++++++++++++++++++++++ ++++++++++++++++++++++++++++++++++
As a record how I understand this, I put the answer here:

evaluate() is defined in

Code:

src/OpenFOAM/fields/GeometricFields/GeometricField/GeometricBoundaryField.C

The structure is:

Code:

template<class Type, template<class> class PatchField, class GeoMesh>
void Foam::GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::
evaluate()
{
    if (debug)
    {
        Info<< "GeometricField<Type, PatchField, GeoMesh>::"
               "GeometricBoundaryField::"
               "evaluate()" << endl;
    }

    if
    (
        Pstream::defaultCommsType == Pstream::blocking
     || Pstream::defaultCommsType == Pstream::nonBlocking
    )
    {
        label nReq = Pstream::nRequests();

        forAll(*this, patchi)
        {
            this->operator[](patchi).initEvaluate(Pstream::defaultCommsType);
        }

        // Block for any outstanding requests
        if
        (
            Pstream::parRun()
         && Pstream::defaultCommsType == Pstream::nonBlocking
        )
        {
            Pstream::waitRequests(nReq);
        }

        forAll(*this, patchi)
        {
            this->operator[](patchi).evaluate(Pstream::defaultCommsType);
        }
    }
    else if (Pstream::defaultCommsType == Pstream::scheduled)
    {
        const lduSchedule& patchSchedule =
            bmesh_.mesh().globalData().patchSchedule();

        forAll(patchSchedule, patchEvali)
        {
            if (patchSchedule[patchEvali].init)
            {
                this->operator[](patchSchedule[patchEvali].patch)
                    .initEvaluate(Pstream::scheduled);
            }
            else
            {
                this->operator[](patchSchedule[patchEvali].patch)
                    .evaluate(Pstream::scheduled);
            }
        }
    }
    else
    {
        FatalErrorIn("GeometricBoundaryField::evaluate()")
            << "Unsuported communications type "
            << Pstream::commsTypeNames[Pstream::defaultCommsType]
            << exit(FatalError);
    }
}

openfoammaofnepo · April 10, 2014, 07:32

Dear Dr Jasak,

The second item you mentioned:

Code:

updateCoeffs()

is just to set the bool quantity update() to be true, no any math manipulations are done in this function. Is my understanding correct?

OFFO

Quote:

Originally Posted by hjasak

Easy:
- on correctBoundaryConditions() for a field
- on updateCoeffs() at matrix creation

correctBoundaryConditions is also called after the linear solver call automatically.

Enjoy,

Hrv

peteryuan · April 16, 2014, 18:54

my understanding so far is:

Those BC types that need updating and evaluation at each time step, they either have updateCoeffs() or evaluate() in the class definition, virtual of course.
When a fvMatrix<type> Eqn is created, the updateCoeffs() is called in its constructor. Then in Eqn().solve() the function correctBoundaryConditions() is called, which contains evaluate().
Now the two functions are implemented differently in every BC, and the solver would also execute different things out according to each BC type defined.

Thanks for corrections and improvement.
peter

abtinansari · December 19, 2014, 02:26

My understanding is that functions like updateCoeffs() and evaluate() are defined first in the upper code level virtually like in GeometricBoundaryField.C and overloaded(redefined) later in specific derived classes where actual math manipulation is done. For example lets look at fixedGradientFvPatchField.C in /src/finiteVolume/fields/fvPatchFields/basic/fixedGradient :

template<class Type>
void fixedGradientFvPatchField<Type>::evaluate(const Pstream::commsTypes)
{
if (!this->updated())
{
this->updateCoeffs();
}

Field<Type>:

perator=
(
this->patchInternalField() + gradient_/this->patch().deltaCoeffs()
);

fvPatchField<Type>::evaluate();
}

Here , the value is updated based on specified gradient in BC file. Can somebody please verify since I'm I also new to C++?

openfoammaofnepo · December 19, 2014, 13:38

I think what you said is correct.

Quote:

Originally Posted by abtinansari

My understanding is that functions like updateCoeffs() and evaluate() are defined first in the upper code level virtually like in GeometricBoundaryField.C and overloaded(redefined) later in specific derived classes where actual math manipulation is done. For example lets look at fixedGradientFvPatchField.C in /src/finiteVolume/fields/fvPatchFields/basic/fixedGradient :

template<class Type>
void fixedGradientFvPatchField<Type>::evaluate(const Pstream::commsTypes)
{
if (!this->updated())
{
this->updateCoeffs();
}

Field<Type>:

perator=
(
this->patchInternalField() + gradient_/this->patch().deltaCoeffs()
);

fvPatchField<Type>::evaluate();
}

Here , the value is updated based on specified gradient in BC file. Can somebody please verify since I'm I also new to C++?

kkamau · April 2, 2019, 13:30

How to call updateCoeff on UEqn. I tried UEqn.updateCoeff() but openfoam returned a compiler error

gaza · February 11, 2020, 05:28

Quote:

Originally Posted by openfoammaofnepo

About the updateCoeffs in the turbulentInlet boundary conditions

Code:

OpenFOAM/OpenFOAM-2.1.1/src/finiteVolume/fields/fvPatchFields/derived/turbulentInlet

It has the following specific forms:

Code:

template<class Type>
void turbulentInletFvPatchField<Type>::updateCoeffs()
{
    if (this->updated())
    {
        return;
    }

    if (curTimeIndex_ != this->db().time().timeIndex())
    {
        Field<Type>& patchField = *this;

        Field<Type> randomField(this->size());

        forAll(patchField, facei)
        {
            ranGen_.randomise(randomField[facei]);
        }

        // Correction-factor to compensate for the loss of RMS fluctuation
        // due to the temporal correlation introduced by the alpha parameter.
        scalar rmsCorr = sqrt(12*(2*alpha_ - sqr(alpha_)))/alpha_;

        patchField =
            (1 - alpha_)*patchField
          + alpha_*
            (
                referenceField_
              + rmsCorr*cmptMultiply
                (
                    randomField - 0.5*pTraits<Type>::one,
                    fluctuationScale_
                )*mag(referenceField_)
            );

        curTimeIndex_ = this->db().time().timeIndex();
    }

    fixedValueFvPatchField<Type>::updateCoeffs();
}

In the above mentioned codes, the updateCoeffs() from the fixedValue boundary conditions type is used

Code:

fixedValueFvPatchField<Type>::updateCoeffs();

What is the role of this line? in the source files for fixedValue, I did not find any information about the relevant definitions there. Could anybody share some information about this problem? Thank you so much.

++++++++++++++++++++++++++++++++++++++++++++++++++ ++++++++++++++++++++++++++++++++++++++++++++++++++ ++++++++++++++++++++++++++++++++++
As a record how I understand this, I put the answer here:

evaluate() is defined in

Code:

src/OpenFOAM/fields/GeometricFields/GeometricField/GeometricBoundaryField.C

The structure is:

Code:

template<class Type, template<class> class PatchField, class GeoMesh>
void Foam::GeometricField<Type, PatchField, GeoMesh>::GeometricBoundaryField::
evaluate()
{
    if (debug)
    {
        Info<< "GeometricField<Type, PatchField, GeoMesh>::"
               "GeometricBoundaryField::"
               "evaluate()" << endl;
    }

    if
    (
        Pstream::defaultCommsType == Pstream::blocking
     || Pstream::defaultCommsType == Pstream::nonBlocking
    )
    {
        label nReq = Pstream::nRequests();

        forAll(*this, patchi)
        {
            this->operator[](patchi).initEvaluate(Pstream::defaultCommsType);
        }

        // Block for any outstanding requests
        if
        (
            Pstream::parRun()
         && Pstream::defaultCommsType == Pstream::nonBlocking
        )
        {
            Pstream::waitRequests(nReq);
        }

        forAll(*this, patchi)
        {
            this->operator[](patchi).evaluate(Pstream::defaultCommsType);
        }
    }
    else if (Pstream::defaultCommsType == Pstream::scheduled)
    {
        const lduSchedule& patchSchedule =
            bmesh_.mesh().globalData().patchSchedule();

        forAll(patchSchedule, patchEvali)
        {
            if (patchSchedule[patchEvali].init)
            {
                this->operator[](patchSchedule[patchEvali].patch)
                    .initEvaluate(Pstream::scheduled);
            }
            else
            {
                this->operator[](patchSchedule[patchEvali].patch)
                    .evaluate(Pstream::scheduled);
            }
        }
    }
    else
    {
        FatalErrorIn("GeometricBoundaryField::evaluate()")
            << "Unsuported communications type "
            << Pstream::commsTypeNames[Pstream::defaultCommsType]
            << exit(FatalError);
    }
}

Hi
I am trying to see a value of a variable inside BC.
I tried standard Info statement:

Code:

Info<< "variable = " << variable << endl;

but it does not give any output in log file.
I tried also

Code:

if (debug) 

{ 
  Info<< "GeometricField<Type, PatchField, GeoMesh>::"              
    "GeometricBoundaryField::"
    "evaluate()" << endl; 
}

but it does not work either. Can anybody help?

February 1, 2014, 10:05	How the boundary conditions are called in the OpenFOAM solvers?	#1
openfoammaofnepo Senior Member Join Date: Jan 2013 Posts: 372 Rep Power: 14	Dear All, I was wondering how the boundary conditions subroutines are called ? Let us take an example: Code: OpenFOAM/OpenFOAM-2.1.1/tutorials/compressible/rhoPimpleFoam/les/pitzDaily In the file: Code: U/0 we have the following boundary conditions for the inlet: Code: inlet { type turbulentInlet; referenceField uniform (10 0 0); fluctuationScale (0.02 0.01 0.01); value uniform (10 0 0); } Does anybody know in which part of the solver is calling the turbulentInlet's subroutine? I am asking this questions because I would like to implement my own BC type in openfoam. Thank you in advance! Annier, minh khang, lpz456 and 1 others like this.

February 3, 2014, 01:54		#2
hjasak Senior Member Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,907 Rep Power: 33	Easy: - on correctBoundaryConditions() for a field - on updateCoeffs() at matrix creation correctBoundaryConditions is also called after the linear solver call automatically. Enjoy, Hrv Pascal_doran, fumiya, dkxls and 19 others like this. __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

February 3, 2014, 12:16		#3
openfoammaofnepo Senior Member Join Date: Jan 2013 Posts: 372 Rep Power: 14	Thank you so much, Hrvoje! About the first one, I get it in the Code: src/OpenFOAM/fields/GeometricFields/GeometricField/GeometricField.C I can get the following lines of codes: Code: // Correct the boundary conditions template<class Type, template<class> class PatchField, class GeoMesh> void Foam::GeometricField<Type, PatchField, GeoMesh>:: correctBoundaryConditions() { this->setUpToDate(); storeOldTimes(); boundaryField_.evaluate(); } Here about the function evaluation(), I cannot find where it is defined. In the following source file: Code: src/OpenFOAM/fields/GeometricFields/GeometricField/GeometricField.H It is declared as Code: //- Evaluate boundary conditions void evaluate(); But it is virtual function here. Could you please give me some hints about where it is defined assuming we are still talking about the turbulentInlet? Thank you very much. abtinansari and TeddyL like this.

February 5, 2014, 18:33		#7
openfoammaofnepo Senior Member Join Date: Jan 2013 Posts: 372 Rep Power: 14	Yes, I agree with you. I also did some digging into the source files. But do you know the role of the following lines: Code: fixedValueFvPatchField<Type>::updateCoeffs();

February 20, 2014, 17:02		#9
hjasak Senior Member Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,907 Rep Power: 33	Please read up on virtual functions - this is basic C++ Hrv Annier and minh khang like this. __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

February 5, 2014, 07:50		#5
openfoammaofnepo Senior Member Join Date: Jan 2013 Posts: 372 Rep Power: 14	No Body also interested in this issue?

April 16, 2014, 18:54		#12
peteryuan New Member Y Join Date: Feb 2013 Location: The Earth Posts: 25 Rep Power: 13	my understanding so far is: Those BC types that need updating and evaluation at each time step, they either have updateCoeffs() or evaluate() in the class definition, virtual of course. When a fvMatrix<type> Eqn is created, the updateCoeffs() is called in its constructor. Then in Eqn().solve() the function correctBoundaryConditions() is called, which contains evaluate(). Now the two functions are implemented differently in every BC, and the solver would also execute different things out according to each BC type defined. Thanks for corrections and improvement. peter

December 19, 2014, 02:26		#13
abtinansari New Member Abtin Ansari Join Date: Oct 2014 Posts: 2 Rep Power: 0	My understanding is that functions like updateCoeffs() and evaluate() are defined first in the upper code level virtually like in GeometricBoundaryField.C and overloaded(redefined) later in specific derived classes where actual math manipulation is done. For example lets look at fixedGradientFvPatchField.C in /src/finiteVolume/fields/fvPatchFields/basic/fixedGradient : template<class Type> void fixedGradientFvPatchField<Type>::evaluate(const Pstream::commsTypes) { if (!this->updated()) { this->updateCoeffs(); } Field<Type>:perator= ( this->patchInternalField() + gradient_/this->patch().deltaCoeffs() ); fvPatchField<Type>::evaluate(); } Here , the value is updated based on specified gradient in BC file. Can somebody please verify since I'm I also new to C++? D.R., Annier and lpz456 like this.

April 2, 2019, 13:30		#15
kkamau New Member -- Country other than USA or Canada -- Join Date: Mar 2019 Posts: 3 Rep Power: 7	How to call updateCoeff on UEqn. I tried UEqn.updateCoeff() but openfoam returned a compiler error

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 07:28
[Commercial meshers] exporting boundary conditions with pointwise -> openFoam	ebah6	OpenFOAM Meshing & Mesh Conversion	2	September 16, 2012 17:57
CFX13 Post Periodic interface	EtaEta	CFX	7	December 8, 2011 18:15
New OpenFOAM Forum Structure	jola	OpenFOAM	2	October 19, 2011 07:55
RPM in Wind Turbine	Pankaj	CFX	9	November 23, 2009 05:05