[smart]

Hi all,

I would like to know what is the meaning of the following terms .A(), .H(), .T():

volScalarField AU = UEqn().A()
U = UEqn().H()/AU
fvc::div(nueff()*dev(fvc::grad(U)().T()))

In addition, could somebody tell me what is the meaning of the "dev" function?

Finally, what is the meaning of "&" in the following line:
phi = fvc::interpolate(rho*U) & mesh.Sf();

Is this "phi" in the UEqn is the same as the one in the pEqn?

Thank you very much to help me understand more about these think.

Sylvain

[eelcovv]

Hi Sylvain,

I am not an OpenFoam expert, but just started digging into the code and came op with the same questions. For the first question I can refer to

http://physics.ucsd.edu/students/cou.../Tutorial2.pdf

slide 9, where they summarise

- A() returns the central coefficients of an fvVectorMatrix
- H() returns the H operation source of an fvVectorMatrix
- Sf() returns cell face area vector of an fvMesh
- flux() returns the face flux field from an fvScalarMatrix

This terms are related to the PISO solution algorithm, a short explanation is given in
http://www.ifdmavt.ethz.ch/education...ols_slides.pdf
slide 48.

The & is the mathematic cross product vector operator (usually denoted with X). If you want calculate the flux field through a surface (in this case the mass flow), you should multiply the velocity vector with the vector representing the cell face using a cross product, i.e. phi_f = rho u_f X S_f
As far as I understood phi is always the mass flux field through the cell faces. Please, anybody correct me if I am wrong

Hope this helps,

Regards

Eelco

[eelcovv]

Sorry, the mass flux through a surface is of course given by the inner product between the velocity and the surface face vector, therefore & should represent the inner product vector operator. That by the way leaves me with a question, because with the inner product you get a scalar, not a vector. Is phi a scalar field of a vector field ? Perhaps somebody could explain.
cheers,

Eelco

[mathieu]

Hi,

A few fast answers:

1. phi is a surfaceScalarField that represents the mass flux through each faces. It is used in convective terms.

2. The .T() function returns the transpose of a tensor (grad(U) in this case).

3. The dev function returns the deviatoric part of a tensor.

4. Generally, phi is not exactly the same in both equations (momentum and pressure). In the momentum equation, phi is the corrected flux from the previous iteration/timestep. In the pressure equation, phi is the mass flux without the "pressure contribution":

U = rUA*UEqn.H();
phi = fvc::interpolate(U) & mesh.Sf();

Hope this helps,

Mathieu

[kathrin_kissling]

Mathieu,

you also wanna try to use the Programmers Guide, which can be found under
http://foam.sourceforge.net/doc/Guid...mmersGuide.pdf

This might help a lot.

Best

Kathrin

[smart]

Thank you for answers!

What is the meaning of A() and other therms? Now, I know that A() returns the central coefficients of an fvVectorMatrix, but can someone tell me more about each term to have a better understanding of each one?

Thank you all,

Sylvain

[mathieu]

Hi Sylvain,

You may find answers in many finite volume CFD books. Furthermore, let me suggest you prof Jasak's thesis where the nomenclature is very similar to the one used in OpenFOAM:

http://powerlab.fsb.hr/ped/kturbo/Op...jeJasakPhD.pdf

Regards,

Mathieu

[mkraposhin]

.A() - diagonal elements of matrix
.H() - off-diagonal

ddt(rho U) + div(rho*U*U) - div(nu grad(U)) = - grad(p)

A() U - H() = - grad(p)

.T() - transpose of matrix

& - scalar product

[makaveli_lcf]

Hi all!

Could some one please give more detailed description for flux correction in PISO loop:

phi = (fvc::interpolate(U) & mesh.Sf())
+ fvc::ddtPhiCorr(rUA, U, phi);

How do we get part denoted as "fvc::ddtPhiCorr(rUA, U, phi)"?

My question is regarding implicit pressure resistance for porous media, because there for class porousZone we use tmp<volTensorField> trTU representing rUA in explicit case.
How ddtPhiCorr method should be modified to be able to use volTensorField instead of volScalarField?

Ok, I already have found in http://foam.sourceforge.net/doc/Doxy...8H_source.html

00013 // ddtPhiCorr not well defined for cases with porosity
00014 phi = fvc::interpolate(rho)*(fvc::interpolate(U) & mesh.Sf());

So still waiting for your comments concerning this point.

[mkraposhin]

Originally Posted by makaveli_lcf

Hi all!

Could some one please give more detailed description for flux correction in PISO loop:

phi = (fvc::interpolate(U) & mesh.Sf())
+ fvc::ddtPhiCorr(rUA, U, phi);

How do we get part denoted as "fvc::ddtPhiCorr(rUA, U, phi)"?

My question is regarding implicit pressure resistance for porous media, because there for class porousZone we use tmp<volTensorField> trTU representing rUA in explicit case.
How ddtPhiCorr method should be modified to be able to use volTensorField instead of volScalarField?

Ok, I already have found in http://foam.sourceforge.net/doc/Doxy...8H_source.html

So still waiting for your comments concerning this point.

Hi, i'm not sure i can help, but i'll try.
Suggest your flow to be incompressible, take look at this files (numbered by order of calling in program):

1) OpenFOAM-1.6/src/finiteVolume/finiteVolume/fvc/fvcDdt.C, function ddtPhiCorr(rA, U, phi), lines 106-125

2) OpenFOAM-1.6/src/finiteVolume/finiteVolume/ddtSchemes/EulerDdtScheme/EulerDdtScheme.C, procedure EulerDdtScheme<Type>::fvcDdtPhiCorr(rA, U, phiAbs). lines 372 - 402

3) OpenFOAM-1.6/src/finiteVolume/finiteVolume/ddtSchemes/ddtScheme/ddtScheme.C, procedure ddtScheme<Type>::fvcDdtPhiCoeff(U, phi), lines 138-233

1) Function #1 calls appropriate type of function #2.

2) Function #2 evaluates difference between old value of flux and flux, calculated with old values of velocity. Then, Function #3 is called to calculate value of Kc (see attached file for more explanation)

3) Function #3 evaluates proportion between flux difference (calculated in #2 and given (current) flux values). Proportion should be between some small epsilon and 1 (unity). Evaluated field returned to #2

4) In Function #2, calculated value phi_d multiplied by 1/A, 1/dt and Kc (previous step) and returned.

For more explanations, see attached file

[makaveli_lcf]

Thank you Matvej for such detailed explanations! Now this point is clear for me.
All the best!

[idrama]

Hey foamers!

Could anybody tell me please, how to store the matrices A and H into a file? I would like to have a look. Or is there even a better possibility so see them?

Cheers,

Claus

[kathrin_kissling]

Hello Claus,

have a look into fvMatrix.H its defined there:

volScalarField matrix.A()
tmp< GeometricField< Type,
fvPatchField, volMesh > > matrix.H()


Hope this helps!

Best

Kathrin

[mohsenkh599]

Hi Foamers
I am an amateur and I want to simulate viscoelastic fluids flow, But I am completely confused with OpenFOAM. And a lot of questions arise for me working with this software. Would you possibly answer some of my questions?
1.For implementing a new model (like LPPT) is it sufficient to write a new application in (OpenFOAM/applications) or it is necessary to modify OpenFOAM/src and/or lib and/or etc.
2. Could you possibly send me one or more new application file which you have made it by yourself (a viscoelastic model for instance). Or a detailed help about implementing new models in OpenFOAM?
I do need your help. Please help. That’s for my master thesis.
Best wishes
Mohsen – m.kh.599@gmail.com

[makaveli_lcf]

Mohsen,

first try to read at least User and Programmer guides, that would help you to avoid such questions.

Good luck!

[Ya_Squall2010]

Originally Posted by mkraposhin

Hi, i'm not sure i can help, but i'll try.
Suggest your flow to be incompressible, take look at this files (numbered by order of calling in program):

1) OpenFOAM-1.6/src/finiteVolume/finiteVolume/fvc/fvcDdt.C, function ddtPhiCorr(rA, U, phi), lines 106-125

2) OpenFOAM-1.6/src/finiteVolume/finiteVolume/ddtSchemes/EulerDdtScheme/EulerDdtScheme.C, procedure EulerDdtScheme<Type>::fvcDdtPhiCorr(rA, U, phiAbs). lines 372 - 402

3) OpenFOAM-1.6/src/finiteVolume/finiteVolume/ddtSchemes/ddtScheme/ddtScheme.C, procedure ddtScheme<Type>::fvcDdtPhiCoeff(U, phi), lines 138-233

1) Function #1 calls appropriate type of function #2.

2) Function #2 evaluates difference between old value of flux and flux, calculated with old values of velocity. Then, Function #3 is called to calculate value of Kc (see attached file for more explanation)

3) Function #3 evaluates proportion between flux difference (calculated in #2 and given (current) flux values). Proportion should be between some small epsilon and 1 (unity). Evaluated field returned to #2

4) In Function #2, calculated value phi_d multiplied by 1/A, 1/dt and Kc (previous step) and returned.

For more explanations, see attached file

Hi, mkraposhin

I was wondering where can we find the mathematical derivation of this treatment or justification? Thanks a lot!

[mohsenkh599]

hi
how can I implement following equation in OpenFoam:
tau_=-2*C*(d(phi)/d(C))
I mean the derivative of phi (a variable) relative to C (a matrix)
the best

[mohsenkh599]

hello again
when compiling a code I get the following message :

mohsen@mohsen-laptop:~/OpenFOAM/OpenFOAM-1.6/src/transportModels$ ./Allwmake
+ wmake libso incompressible
'/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libincompressibleTransportModels.so' is up to date.
+ wmake libso interfaceProperties
'/home/mohsen/OpenFOAM/OpenFOAM-1.6/lib/linuxGccDPOpt/libinterfaceProperties.so' is up to date.
+ wmake libso viscoelastic
wmakeLnInclude: linking include files to ./lnInclude
make: *** No rule to make target `viscoelasticLaws/Conf/Conf.dep', needed by `Make/linuxGccDPOpt/dependencies'. Stop.
mohsen@mohsen-laptop:~/OpenFOAM/OpenFOAM-1.6/src/transportModels$


whats the problem?
the code is as follows:

#include "Conf.H"
#include "addToRunTimeSelectionTable.H"

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

namespace Foam
{

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

defineTypeNameAndDebug(Conf, 0);
addToRunTimeSelectionTable(viscoelasticLaw, Conf, dictionary);

// * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * //

// from components
Conf::Conf
(
const word& name,
const volVectorField& U,
const surfaceScalarField& phi,
const dictionary& dict
)
:
viscoelasticLaw(name, U, phi),
C_
(
IOobject
(
"C" + name,
U.time().timeName(),
U.mesh(),
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
U.mesh()
),
tau_
(
IOobject
(
"tau" + name,
U.time().timeName(),
U.mesh(),
IOobject::NO_READ,
IOobject::AUTO_WRITE
),
U.mesh(),
dimensionedSymmTensor
(
"zero",
dimensionSet(1, -1, -2, 0, 0, 0, 0),
symmTensor::zero
)
),
I_
(
dimensionedSymmTensor
(
"I",
dimensionSet(0, 0, 0, 0, 0, 0, 0),
symmTensor
(
1, 0, 0,
1, 0,
1
)
)
),
rho_(dict.lookup("rho")),
etaS_(dict.lookup("etaS")),
etaP_(dict.lookup("etaP")),
M_(dict.lookup("M")),
lambda_(dict.lookup("lambda")),
{}


// * * * * * * * * * *t * * * * * Member Functions * * * * * * * * * * * * * //

tmp<fvVectorMatrix> Conf::divTau(volVectorField& U) const
{

dimensionedScalar etaPEff = etaP_;

return
(
fvc::div(tau_/rho_, "div(tau)")
- fvc::laplacian(etaPEff/rho_, U, "laplacian(etaPEff,U)")
+ fvm::laplacian( (etaPEff + etaS_)/rho_, U, "laplacian(etaPEff+etaS,U)")
);

}


void Conf::correct()
{
// Velocity gradient tensor
volTensorField L = fvc::grad( U() );
// Transpose of grad(U)
volTensorField LT = fvc::L.T();
// Twice the rate of deformation tensor
volSymmTensorField twoD = twoSymm( L );
// C . gamma
volTensorField moh1 = twoD & C_;
// gamma . C
volTensorField moh2 = C_ & twoD;
// vorticity
volTensorField vor = L - LT;
//
volTensorField moh3 = vor & C_;
//
volTensorField moh3 = C & vor;


// Evolution of orientation
tmp<fvSymmTensorMatrix> tauEqn
(
fvm::ddt(tau_)
==
1/4*(moh1+moh2)
-1/4*(moh3+moh4)
);

tauEqn().relax();
solve(tauEqn);

// Evolution of the backbone stretch
tmp<fvScalarMatrix> pheeEqn
(
phee
==
(lambda/2)*Foam::sqr(tr((I - inv(C))/2))
+ M*Foam::sqr(tr((I - inv(C))/2))
);

pheeEqn().relax();
solve(pheeEqn);

// Viscoelastic stress
tau_ = -2*C_*fvm::ddt(C);

}


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

} // End namespace Foam

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

thank you very much

[flowris]

A little suggestion: sometimes people forget to run "wclean" before "wmake", provoking the error you had.

[RuiVO]

Hello Foamers. This thread is a very usefull one indeed. I still have two questions though.
Why is it written :

dev2(fvc::grad(U)().T()) instead of dev2(fvc::grad(U).T())

Why the extra pair of parenthesis ??

The other question is what is the meaning of "twoSymm" in the following expression:

dev(twoSymm(fvc::grad(U_)))

Best Regards

Rui