Trying to understand outletInlet BC

ThomasV · December 9, 2014, 09:45

Hi!

I have some problems understanding how exactly the outletInlet BC works. What is done in its class is this:

Code:

template<class Type>
void Foam::outletInletFvPatchField<Type>::updateCoeffs()
{
// this exits the method if the updateCoeffs() method  already did run... 
// Out of curiosity: where exactly is this switched  back to false again?
    if (this->updated()) 
    {
        return;
    }

// this creates the phip fvsPatchField (I guess the "p" stands for phi_patch)
// the flux in the patch node is assigned to phip
    const fvsPatchField<scalar>& phip =
        this->patch().template lookupPatchField<surfaceScalarField, scalar>
        (
            phiName_
        );

// This assigns the absolute value of phip to the valueFraction w
    this->valueFraction() = pos(phip);

// this basically just sets updated() to true
    mixedFvPatchField<Type>::updateCoeffs();
}

I now don't really get how this is supposed to be the entire outletInlet condition with its differentiation between a flux out of the domain and into the domain. All that really happens is that the valueFraction w gets a new value. This also is the only difference between the outletInlet and inletOutlet BC as for the inletOutlet case one just has this:

Code:

    this->valueFraction() = 1.0 - pos(phip);

So this valueFraction() variable w is derived from the mixedFvPatchField class. Its description says that this is what's meant to be calculated:

$x_p = w \cdot x_p + (1-w) \left(x_c + \frac{\nabla_\perp x}{\Delta}\right)$

With

= patch value although I think the second

that's multiplied with

should have gotten a variable name of its own as it's the constant number from the Dirichlet boundary condition if I got this right while the initial

stands for the patch node value which is a mix of the Dirichlet and Neumann BC

= cell value

= weight field i.e. valueFraction
$\Delta$ = inverse distance cell center <-> cell face where the patch is

This can be found in the mixedFvPatchField's operator= method:

Code:

    Field<Type>::operator=
    (
        valueFraction_*refValue_
      +
        (1.0 - valueFraction_)*
        (
            this->patchInternalField()
          + refGrad_/this->patch().deltaCoeffs()
        )
    );

Can someone explain to me how this is supposed to work as a inlet/outlet condition? I mean the mixedFvPatchField BC has this mixture between the constant Dirichlet BC and a gradient Neumann BC via this sum and the weight factor w deciding how much of which of the two BC conditions gets accounted for. But how does taking the absolute value of phi and make it the new w and why is phip always in the 0-1 range needed for w? I still don't really get that part...

I would have expected some if-statements checking whether the flux goes inside or outside the domain and then some appropiate calculations depending on the case...

It would be nice if someone could give me some hints to understand the idea behind the given approach as I don't get why making the flux the valueFraction solves the problem...

alexeym · December 9, 2014, 09:59

Hi,

You're not quite correct about

Code:

// This assigns the absolute value of phip to the valueFraction w
    this->valueFraction() = pos(phip);

See definition of pos function (for scalar)

Code:

inline Scalar pos(const Scalar s)
{
    return (s >= 0)? 1: 0;
}

So as it is described in outletInletFvPatchField.H

Code:

    Sign conventions:
    - positive flux (out of domain): apply the user-specified fixed value
    - negative flux (into of domain): apply zero-gradient condition

ThomasV · December 9, 2014, 10:11

Ah I see - so pos(x) and neg(x) are meant as booleans. I had thought they'd just let you change the sign of a number to either a positive or negative one...

Thanks for clarifying this!

ThomasV · January 14, 2015, 08:43

So now I'm having another question concerning this method / equation I already did mention:

Code:

    Field<Type>::operator=
    (
        valueFraction_*refValue_
      +
        (1.0 - valueFraction_)*
        (
            this->patchInternalField()
          + refGrad_/this->patch().deltaCoeffs()
        )
    );

Is there a possibility to include terms for let's say a cell value? I basically want to change the given equation to serve my needs and for this I need to grab e.g. the pressure value of the cell neighboring the patch. I tried doing it the same way as the outletInlet BC reads the value for phi but the expressions I'm trying to use are incorrect at this position in the code. Did someone else already solve a similar problem or is there maybe a BC which reads and uses cell values so I can have a look at that?

Linse · January 14, 2015, 08:52

It is a long shot, but there is some reading of closeby fields within the mixed-BCs, e.g. the wallHeatTransfer-BC. MAYBE that gives further clues where you could proceed looking for a solution to your question/problem?

alexeym · January 14, 2015, 09:39

Hi,

1. There's fixedInternalValueFvPatchField. It accesses internal field.

2. There's totalPressure BC. It is BC for pressure and it accesses patch values of velocity.

3. And finally there's, for example, flowRateInletVelocity, and here's how it accesses rho volume field:

Code:

...
        // mass flow-rate
        if (db().foundObject<volScalarField>(rhoName_))
        {
            const fvPatchField<scalar>& rhop =
                patch().lookupPatchField<volScalarField, scalar>(rhoName_);

            operator==(n*avgU/rhop);
        }
...

ThomasV · January 14, 2015, 12:00

Thanks for your suggestions - I'll have a look at them!

ThomasV · January 19, 2015, 13:35

So I had some time to work on the BC again and while I can reproduce the examples mentioned here those just give me the patch values via the "lookupPatchField" method. I need to use the internal cell values though. The "patchInternalField" function seems to do just that but I can't figure out how to tell OpenFOAM which field it should read from. I found some examples where a simple "this->patchInternalField()"; is used but if I got this right this is just about reading the values for the property you applied the BC to. The function itself asks for a "UList" but I didn't find any examples yet which might give me a clue how to read the values of a specific field of my choice...

Any suggestions on that? Does "patchInternalField" give me the needed functionality after all? It might not be able to read a "named field" after all but if that's the case I don't see how to read a cell value of my choice after all as the fvPatch class doesn't seem to deliver another interesting method meant for a purpose like this...

alexeym · January 20, 2015, 04:05

Hi,

Maybe I did not quite get your question but...

1. What is wrong with the example no. 3 from my last post? It will provide you with the patch field of any other volume fiend.

2. Also you have another way, maybe it is not quite idiomatic. Every fvPatchField has db() method, which returns constant reference to objectRegistry. Through this object you can lookup volume fields (lookupObject<Type>("field name")). Also fvPatchField has patch() method, which returns constant reference to fvPatch object, which has faceCells() method. So you can lookup volume field you need, then iterate over faces of the patch, use faceCells() to find face-cell correspondence and extract value using cell index.

ThomasV · January 20, 2015, 04:57

Well I basically created a clone of the outletInlet BC (together with a custom mixedFvPatchField) and what it does is that upon starting my solver the variable in the style of example #3 gets initialized and also has the value of the internal cell. In the course of the solving process its values won't get updated though. In order to test this I created a new field that isn't used anywhere but for a simple function that increases its value by 1 in every timestep. When using "Info" commands to print the values the BC condition always will tell...

TempBC = type calculated; value uniform 1400;

... while the actual Temp volume field is increased in every timestep and e.g. will lead to:

internalField uniform 1434;

1400 was the value I assigned in the createFields.H:

Code:

    volScalarField Temp
    (
        IOobject
        (
            "Temp",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimensionSet(0, 0, 0, 1, 0, 0, 0), 1400)
    );

That's why I think that the lookupPatchField function might work for initializing but afterwards it just sticks to this value and doesn't adapt to changes in the respective field. I'll check for some problems in the general BC logic though which might prevent an update...

alexeym · January 20, 2015, 05:10

Hi,

Unfortunately I did not get what was updated, why it should be updated etc.

Can you post the code of your modified BC? Can you post a code of modified solver (you just do Temp = Temp + dimensionedScalar("One", dimTemperature, 1) on every timestep?)?

ThomasV · January 20, 2015, 09:54

Well my approach was to mimic the behaviour of the outletInlet BC just with my own function in an altered mixedFVPatchField BC (c.f. formula from the opening posting here). There I made some additions in order to create objects which should read certain cell values (adjacent to the patch). I put them into the evaluate function of the former mixedFvPatchField which now looks like this:

Code:

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

                  const fvPatchField<scalar>& TempBC =
                this->patch().template lookupPatchField<volScalarField, scalar>(TempName_);
                
                const fvPatchField<scalar>& TestFieldBC =
                this->patch().template lookupPatchField<volScalarField, scalar>(TestFieldName_);
    
        Info << "TempBC = " << TempBC << endl;
        Info << "TestFieldBC= " << TestFieldBC << endl;
                
                
    Field<Type>::operator=
    (
        
        valueFraction_*refValue_
      +
        (1.0 - valueFraction_)* TempBC * TestFieldBC *
        (
            this->patchInternalField()
          + refGrad_/this->patch().deltaCoeffs()
        )
    );

    fvPatchField<Type>::evaluate();
}

Basically the method from example #3 for two fields I want to read values from and with an Info command printing out their respective values to the log file. I also added them to the operator= function in order to test if the compiler accepts the objects there. I use this BC on an interFoam solver where the case consist of just one single cell and my new outletInlet BC is applied to one of the cell's sides - i.e. it's applied to alpha...

I of course also added the needed words for the two fields to the mixedField's constructors which I won't list here now...

The two fields themselves are created via the createFields.H file like this:

Code:

    Info<< "Initializing temperature field >>Temp<<\n" << endl;
    volScalarField Temp
    (
        IOobject
        (
            "Temp",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimensionSet(0, 0, 0, 1, 0, 0, 0), 1400)
    );
    
    
    Info<< "Initializing field >>TestField<<\n" << endl;
    volScalarField TestField
    (
        IOobject
        (
            "TestField",
            runTime.timeName(),
            mesh,
            IOobject::NO_READ, // values are calculated and thus needn't an initial case file with start values
            IOobject::AUTO_WRITE
        ),
        mesh,
        dimensionedScalar("zero", dimensionSet(0, 0, 0, 0, 0, 0, 0), 9999.0)
    );

So far things worked fine and I now wanted to check if my objects from the boundary condition update their values. For this purpose I added the following code to the end of the runtime loop so it gets executed once for each timestep:

Code:

        forAll(Temp, celli)
        {
            Temp[celli] = Temp[celli] + 1;
        }
        
        Info << "Temp = " << Temp << endl;

So what happens is that each timestep that becomes calculated adds "1" to the value of "Temp" starting with its initial value of 1400...
Well what else is there to say? My BC is applied to one wall for alpha like this:

Code:

    rightWall
    {
 
        type            diffPressOutletInlet;
        phi             phi;        // name of flux field (default = phi)
        outletValue     uniform 0;  // reverse flow (inlet) value
        value           uniform 0;  // initial value
    }

It's just an unaltered outletInlet BC using my custom mixedFvPatchField instead of the original one. My problem now is that the values for the objects in the boundary condition won't update - they stay at 1400 while my Temp actually increases with every timestep. Here an excerpt from my logfile:

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PIMPLE: Operating solver in PISO mode

Reading field p_rgh

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar

Reading g
Calculating field g.h

No finite volume options present

Initializing temperature field >>Temp<<

Initializing field >>TestField<<

time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG:  Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
Interface Courant Number mean: 0 max: 0
deltaT = 0.00119048
Time = 0.00119048

smoothSolver:  Solving for alpha.water, Initial residual = 0, Final residual = 0, No Iterations 0
TempBC = type            calculated;
value           uniform 1400;

TestFieldBC= type            calculated;
value           uniform 9999;

Phase-1 volume fraction = 0  Min(alpha1) = 0  Max(alpha1) = 0
MULES: Correcting alpha.water
TempBC = type            calculated;
value           uniform 1400;

TestFieldBC= type            calculated;
value           uniform 9999;

MULES: Correcting alpha.water
TempBC = type            calculated;
value           uniform 1400;

TestFieldBC= type            calculated;
value           uniform 9999;

Phase-1 volume fraction = 0  Min(alpha1) = 0  Max(alpha1) = 0
DICPCG:  Solving for p_rgh, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG:  Solving for p_rgh, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG:  Solving for p_rgh, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
Temp = dimensions      [0 0 0 1 0 0 0];

internalField   uniform 1401;

boundaryField
{
    leftWall
    {
        type            calculated;
        value           uniform 1400;
    }
    rightWall
    {
        type            calculated;
        value           uniform 1400;
    }
    lowerWall
    {
        type            calculated;
        value           uniform 1400;
    }
    upperWall
    {
        type            calculated;
        value           uniform 1400;
    }
    defaultFaces
    {
        type            empty;
    }
}

ExecutionTime = 0 s  ClockTime = 0 s

Courant Number mean: 0 max: 0
Interface Courant Number mean: 0 max: 0
deltaT = 0.00141156
Time = 0.00260204

smoothSolver:  Solving for alpha.water, Initial residual = 0, Final residual = 0, No Iterations 0
TempBC = type            calculated;
value           uniform 1400;

TestFieldBC= type            calculated;
value           uniform 9999;

Phase-1 volume fraction = 0  Min(alpha1) = 0  Max(alpha1) = 0
MULES: Correcting alpha.water
TempBC = type            calculated;
value           uniform 1400;

TestFieldBC= type            calculated;
value           uniform 9999;

MULES: Correcting alpha.water
TempBC = type            calculated;
value           uniform 1400;

TestFieldBC= type            calculated;
value           uniform 9999;

Phase-1 volume fraction = 0  Min(alpha1) = 0  Max(alpha1) = 0
DICPCG:  Solving for p_rgh, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG:  Solving for p_rgh, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
DICPCG:  Solving for p_rgh, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
Temp = dimensions      [0 0 0 1 0 0 0];

internalField   uniform 1402;

boundaryField
{
    leftWall
    {
        type            calculated;
        value           uniform 1400;
    }
    rightWall
    {
        type            calculated;
        value           uniform 1400;
    }
    lowerWall
    {
        type            calculated;
        value           uniform 1400;
    }
    upperWall
    {
        type            calculated;
        value           uniform 1400;
    }
    defaultFaces
    {
        type            empty;
    }
}

ExecutionTime = 0 s  ClockTime = 0 s

alexeym · January 20, 2015, 10:25

Well, (maybe) my bad,

Code:

const fvPatchField<scalar>& rhop =
                patch().lookupPatchField<volScalarField, scalar>(rhoName_);

returns fvPatchField i.e. value on the patch. As in the code you update only internal field of Temp and TestField, on the patch you still get initial value specified by value key in BC's dictionary.

There's still a way I've described in the last message. And it is actually implemented in Foam::fvPatch::patchInternalField method.

I.e. your code should look like:

Code:

const label patchi = patch().index();
const volScalarField Temp = db().lookupObject<volScalarField>(TempName_);
const scalarField TempIntF(Temp.boundaryField()[patchi].patchInternalField());

Info<< TempIntF << endl;

See for example nutUTabulatedWallFunctionFvPatchScalarField::calcN ut() in src/TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUTabulatedWallFunction/nutUTabulatedWallFunctionFvPatchScalarField.C.

ThomasV · January 21, 2015, 12:08

Well due to all the template stuff used in the fvPatchField things are a bit more complicated here. Using your code results in this error:

Code:

diffPressBC/diffPressFvPatchField.C: In member function ‘virtual void Foam::diffPressFvPatchField<Type>::evaluate(Foam::UPstream::commsTypes)’:
diffPressBC/diffPressFvPatchField.C:188:28: error: there are no arguments to ‘patch’ that depend on a template parameter, so a declaration of ‘patch’ must be available [-fpermissive]
 const label patchi = patch().index();
                            ^
diffPressBC/diffPressFvPatchField.C:188:28: note: (if you use ‘-fpermissive’, G++ will accept your code, but allowing the use of an undeclared name is deprecated)
diffPressBC/diffPressFvPatchField.C:189:32: error: there are no arguments to ‘db’ that depend on a template parameter, so a declaration of ‘db’ must be available [-fpermissive]
 const volScalarField Temp = db().lookupObject<volScalarField>(TempName_);
                                ^
diffPressBC/diffPressFvPatchField.C:189:61: error: expected primary-expression before ‘>’ token
 const volScalarField Temp = db().lookupObject<volScalarField>(TempName_);
                                                             ^
diffPressBC/diffPressFvPatchField.C:190:32: error: invalid use of incomplete type ‘const volScalarField {aka const class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’
 const scalarField TempIntF(Temp.boundaryField()[patchi].patchInternalField());
                                ^
In file included from /opt/OpenFOAM-2.3.0/src/finiteVolume/lnInclude/surfaceInterpolation.H:40:0,
                 from /opt/OpenFOAM-2.3.0/src/finiteVolume/lnInclude/fvMesh.H:54,
                 from /opt/OpenFOAM-2.3.0/src/finiteVolume/lnInclude/fvPatchField.C:28,
                 from /opt/OpenFOAM-2.3.0/src/finiteVolume/lnInclude/fvPatchField.H:588,
                 from diffPressBC/diffPressFvPatchField.H:75,
                 from diffPressBC/diffPressFvPatchFields.H:29,
                 from diffPressBC/diffPressFvPatchFields.C:26:
/opt/OpenFOAM-2.3.0/src/finiteVolume/lnInclude/volFieldsFwd.H:52:7: error: declaration of ‘const volScalarField {aka const class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’
 class GeometricField;

I tried changing the first two lines into this:

Code:

const label patchi = this->patch().template index();
const volScalarField Temp = this->db().template lookupObject<volScalarField>(TempName_);

This results in some long compiler notes but in the end these just seem to be complicated and numerous "unused variable" warnings without an error. I'm not sure though if e.g. just defining a constant volScalarField the way I did it is a valid approach even though it gives no error (yet)...

I wasn't able to find a sound formulation for the final line of your code though...

alexeym · January 21, 2015, 12:21

Hi,

Yes, I forgot & after volScalarField in the code. Surely you do not need to create copy of the volScalarField, reference should be enough. So code shall be something like:

Code:

const label patchi = this->patch().template index();
const volScalarField& Temp = this->db().template lookupObject<volScalarField>(TempName_);

The last line creates constant copy of the field returned by patchInternalField call.

alexeym · January 21, 2015, 12:30

Btw, if you post code here, it'll be easier for me to check my propositions for errors. As currently I'm writing the code quite "theoretically".

ThomasV · January 22, 2015, 06:16

I finally got things working. I dont really understand why but the proposed command...

Code:

const scalarField TempIntF(Temp.boundaryField()[patchi].patchInternalField());

... wont' work. Ok - the "Temp" should be "Temp()" but the compiler keeps telling me it doesn't know how to call it...

As a workaround I just skipped the definition of the volScalarField Temp and did put everything into TempIntF:

Code:

const scalarField TempIntF = this->db().template lookupObject<volScalarField>(TempName_).boundaryField()[patchi].patchInternalField();

This works...

alexeym · January 22, 2015, 06:22

Good to know.

Still I do not get why Temp should be Temp(), was not able to find definition of () operator neither for GeometricField (which volScalarField is), nor for its parents.

Also not quite get why do you need template BC instead of just fvPatchScalarField as your BC is for pressure (deducing it from the name

)

ThomasV · January 22, 2015, 07:43

Well when you don't add template code you get an error like this (if I got right what you wanted to express):

Code:

error: there are no arguments to ‘db’ that depend on a template parameter, so a declaration of ‘db’ must be available [-fpermissive]

Concerning Temp() instead of just Temp - I found someone talking about using it this way. When trying to do it your way you get this error:

Code:

error: invalid use of incomplete type ‘const volScalarField {aka const class Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>}’
 const scalarField TempIntF2(Temp.boundaryField()[patchi].patchInternalField());
                                 ^
In file included from /opt/OpenFOAM-2.3.0/src/finiteVolume/lnInclude/surfaceInterpolation.H:40:0,

alexeym · January 22, 2015, 08:57

Well, I understand why you need to add template to your code, I do not understand why diffPressFvPatchField should be template. Whole BC is template (that means you plan to use BC for scalars, vectors, tensors etc.), while according to the name you plan to use it for pressure (which is scalar).

Concerning your

Code:

error: invalid use of incomplete type

can you show your include section of the code?

December 9, 2014, 09:45	Trying to understand outletInlet BC	#1
ThomasV Member Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 13	Hi! I have some problems understanding how exactly the outletInlet BC works. What is done in its class is this: Code: template<class Type> void Foam::outletInletFvPatchField<Type>::updateCoeffs() { // this exits the method if the updateCoeffs() method already did run... // Out of curiosity: where exactly is this switched back to false again? if (this->updated()) { return; } // this creates the phip fvsPatchField (I guess the "p" stands for phi_patch) // the flux in the patch node is assigned to phip const fvsPatchField<scalar>& phip = this->patch().template lookupPatchField<surfaceScalarField, scalar> ( phiName_ ); // This assigns the absolute value of phip to the valueFraction w this->valueFraction() = pos(phip); // this basically just sets updated() to true mixedFvPatchField<Type>::updateCoeffs(); } I now don't really get how this is supposed to be the entire outletInlet condition with its differentiation between a flux out of the domain and into the domain. All that really happens is that the valueFraction w gets a new value. This also is the only difference between the outletInlet and inletOutlet BC as for the inletOutlet case one just has this: Code: this->valueFraction() = 1.0 - pos(phip); So this valueFraction() variable w is derived from the mixedFvPatchField class. Its description says that this is what's meant to be calculated: $x_p = w \cdot x_p + (1-w) \left(x_c + \frac{\nabla_\perp x}{\Delta}\right)$ With = patch value although I think the second that's multiplied with should have gotten a variable name of its own as it's the constant number from the Dirichlet boundary condition if I got this right while the initial stands for the patch node value which is a mix of the Dirichlet and Neumann BC = cell value = weight field i.e. valueFraction $\Delta$ = inverse distance cell center <-> cell face where the patch is This can be found in the mixedFvPatchField's operator= method: Code: Field<Type>::operator= ( valueFraction_refValue_ + (1.0 - valueFraction_) ( this->patchInternalField() + refGrad_/this->patch().deltaCoeffs() ) ); Can someone explain to me how this is supposed to work as a inlet/outlet condition? I mean the mixedFvPatchField BC has this mixture between the constant Dirichlet BC and a gradient Neumann BC via this sum and the weight factor w deciding how much of which of the two BC conditions gets accounted for. But how does taking the absolute value of phi and make it the new w and why is phip always in the 0-1 range needed for w? I still don't really get that part... I would have expected some if-statements checking whether the flux goes inside or outside the domain and then some appropiate calculations depending on the case... It would be nice if someone could give me some hints to understand the idea behind the given approach as I don't get why making the flux the valueFraction solves the problem...

January 14, 2015, 08:43		#4
ThomasV Member Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 13	So now I'm having another question concerning this method / equation I already did mention: Code: Field<Type>::operator= ( valueFraction_refValue_ + (1.0 - valueFraction_) ( this->patchInternalField() + refGrad_/this->patch().deltaCoeffs() ) ); Is there a possibility to include terms for let's say a cell value? I basically want to change the given equation to serve my needs and for this I need to grab e.g. the pressure value of the cell neighboring the patch. I tried doing it the same way as the outletInlet BC reads the value for phi but the expressions I'm trying to use are incorrect at this position in the code. Did someone else already solve a similar problem or is there maybe a BC which reads and uses cell values so I can have a look at that?

January 14, 2015, 08:52	Long shot...	#5
Linse Senior Member Bernhard Linseisen Join Date: May 2010 Location: Heilbronn Posts: 183 Blog Entries: 1 Rep Power: 16	It is a long shot, but there is some reading of closeby fields within the mixed-BCs, e.g. the wallHeatTransfer-BC. MAYBE that gives further clues where you could proceed looking for a solution to your question/problem?

January 14, 2015, 09:39		#6
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Hi, 1. There's fixedInternalValueFvPatchField. It accesses internal field. 2. There's totalPressure BC. It is BC for pressure and it accesses patch values of velocity. 3. And finally there's, for example, flowRateInletVelocity, and here's how it accesses rho volume field: Code: ... // mass flow-rate if (db().foundObject<volScalarField>(rhoName_)) { const fvPatchField<scalar>& rhop = patch().lookupPatchField<volScalarField, scalar>(rhoName_); operator==(n*avgU/rhop); } ...

January 20, 2015, 04:57		#10
ThomasV Member Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 13	Well I basically created a clone of the outletInlet BC (together with a custom mixedFvPatchField) and what it does is that upon starting my solver the variable in the style of example #3 gets initialized and also has the value of the internal cell. In the course of the solving process its values won't get updated though. In order to test this I created a new field that isn't used anywhere but for a simple function that increases its value by 1 in every timestep. When using "Info" commands to print the values the BC condition always will tell... TempBC = type calculated; value uniform 1400; ... while the actual Temp volume field is increased in every timestep and e.g. will lead to: internalField uniform 1434; 1400 was the value I assigned in the createFields.H: Code: volScalarField Temp ( IOobject ( "Temp", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::AUTO_WRITE ), mesh, dimensionedScalar("zero", dimensionSet(0, 0, 0, 1, 0, 0, 0), 1400) ); That's why I think that the lookupPatchField function might work for initializing but afterwards it just sticks to this value and doesn't adapt to changes in the respective field. I'll check for some problems in the general BC logic though which might prevent an update...

December 9, 2014, 10:11		#3
ThomasV Member Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 13	Ah I see - so pos(x) and neg(x) are meant as booleans. I had thought they'd just let you change the sign of a number to either a positive or negative one... Thanks for clarifying this!

January 14, 2015, 12:00		#7
ThomasV Member Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 13	Thanks for your suggestions - I'll have a look at them!

January 19, 2015, 13:35		#8
ThomasV Member Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 13	So I had some time to work on the BC again and while I can reproduce the examples mentioned here those just give me the patch values via the "lookupPatchField" method. I need to use the internal cell values though. The "patchInternalField" function seems to do just that but I can't figure out how to tell OpenFOAM which field it should read from. I found some examples where a simple "this->patchInternalField()"; is used but if I got this right this is just about reading the values for the property you applied the BC to. The function itself asks for a "UList" but I didn't find any examples yet which might give me a clue how to read the values of a specific field of my choice... Any suggestions on that? Does "patchInternalField" give me the needed functionality after all? It might not be able to read a "named field" after all but if that's the case I don't see how to read a cell value of my choice after all as the fvPatch class doesn't seem to deliver another interesting method meant for a purpose like this...

January 20, 2015, 04:05		#9
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Hi, Maybe I did not quite get your question but... 1. What is wrong with the example no. 3 from my last post? It will provide you with the patch field of any other volume fiend. 2. Also you have another way, maybe it is not quite idiomatic. Every fvPatchField has db() method, which returns constant reference to objectRegistry. Through this object you can lookup volume fields (lookupObject<Type>("field name")). Also fvPatchField has patch() method, which returns constant reference to fvPatch object, which has faceCells() method. So you can lookup volume field you need, then iterate over faces of the patch, use faceCells() to find face-cell correspondence and extract value using cell index.

January 20, 2015, 05:10		#11
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Hi, Unfortunately I did not get what was updated, why it should be updated etc. Can you post the code of your modified BC? Can you post a code of modified solver (you just do Temp = Temp + dimensionedScalar("One", dimTemperature, 1) on every timestep?)?

January 20, 2015, 10:25		#13
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Well, (maybe) my bad, Code: const fvPatchField<scalar>& rhop = patch().lookupPatchField<volScalarField, scalar>(rhoName_); returns fvPatchField i.e. value on the patch. As in the code you update only internal field of Temp and TestField, on the patch you still get initial value specified by value key in BC's dictionary. There's still a way I've described in the last message. And it is actually implemented in Foam::fvPatch::patchInternalField method. I.e. your code should look like: Code: const label patchi = patch().index(); const volScalarField Temp = db().lookupObject<volScalarField>(TempName_); const scalarField TempIntF(Temp.boundaryField()[patchi].patchInternalField()); Info<< TempIntF << endl; See for example nutUTabulatedWallFunctionFvPatchScalarField::calcN ut() in src/TurbulenceModels/turbulenceModels/RAS/derivedFvPatchFields/wallFunctions/nutWallFunctions/nutUTabulatedWallFunction/nutUTabulatedWallFunctionFvPatchScalarField.C.

January 21, 2015, 12:21		#15
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Hi, Yes, I forgot & after volScalarField in the code. Surely you do not need to create copy of the volScalarField, reference should be enough. So code shall be something like: Code: const label patchi = this->patch().template index(); const volScalarField& Temp = this->db().template lookupObject<volScalarField>(TempName_); The last line creates constant copy of the field returned by patchInternalField call.

January 21, 2015, 12:30		#16
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Btw, if you post code here, it'll be easier for me to check my propositions for errors. As currently I'm writing the code quite "theoretically".

January 22, 2015, 06:16		#17
ThomasV Member Thomas Vossel Join Date: Aug 2013 Location: Germany Posts: 45 Rep Power: 13	I finally got things working. I dont really understand why but the proposed command... Code: const scalarField TempIntF(Temp.boundaryField()[patchi].patchInternalField()); ... wont' work. Ok - the "Temp" should be "Temp()" but the compiler keeps telling me it doesn't know how to call it... As a workaround I just skipped the definition of the volScalarField Temp and did put everything into TempIntF: Code: const scalarField TempIntF = this->db().template lookupObject<volScalarField>(TempName_).boundaryField()[patchi].patchInternalField(); This works...

January 22, 2015, 06:22		#18
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Good to know. Still I do not get why Temp should be Temp(), was not able to find definition of () operator neither for GeometricField (which volScalarField is), nor for its parents. Also not quite get why do you need template BC instead of just fvPatchScalarField as your BC is for pressure (deducing it from the name )

January 22, 2015, 08:57		#20
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,938 Rep Power: 39	Well, I understand why you need to add template to your code, I do not understand why diffPressFvPatchField should be template. Whole BC is template (that means you plan to use BC for scalars, vectors, tensors etc.), while according to the name you plan to use it for pressure (which is scalar). Concerning your Code: error: invalid use of incomplete type can you show your include section of the code?