
[Sponsors] 
November 24, 2009, 16:28 
Programming questions

#1 
Member
Sylvain Martel
Join Date: Apr 2009
Location: University of Sherbrooke/Quebec/Canada
Posts: 51
Rep Power: 8 
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 

November 24, 2009, 23:25 

#2 
Senior Member
Eelco van Vliet
Join Date: Mar 2009
Location: The Netherlands
Posts: 122
Rep Power: 9 
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 

November 24, 2009, 23:48 
correction

#3 
Senior Member
Eelco van Vliet
Join Date: Mar 2009
Location: The Netherlands
Posts: 122
Rep Power: 9 
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 

November 25, 2009, 00:19 

#4 
Member
Mathieu Olivier
Join Date: Mar 2009
Location: Quebec City, Canada
Posts: 76
Rep Power: 8 
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 

November 25, 2009, 03:55 

#5 
Senior Member
Kathrin Kissling
Join Date: Mar 2009
Location: Besigheim, Germany
Posts: 134
Rep Power: 8 
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 

November 25, 2009, 15:49 

#6 
Member
Sylvain Martel
Join Date: Apr 2009
Location: University of Sherbrooke/Quebec/Canada
Posts: 51
Rep Power: 8 
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 

November 25, 2009, 15:59 

#7 
Member
Mathieu Olivier
Join Date: Mar 2009
Location: Quebec City, Canada
Posts: 76
Rep Power: 8 
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 

December 3, 2009, 12:28 

#8 
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
.A()  diagonal elements of matrix
.H()  offdiagonal ddt(rho U) + div(rho*U*U)  div(nu grad(U)) =  grad(p) A() U  H() =  grad(p) .T()  transpose of matrix &  scalar product 

January 6, 2010, 09:45 

#9  
Senior Member

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 Quote:
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben FranzJosefStr. 18 A  8700 Leoben Österreich / Austria Tel.: +43 3842  402  3125 http://smmp.unileoben.ac.at Last edited by makaveli_lcf; January 6, 2010 at 10:14. 

January 11, 2010, 16:27 

#10  
Senior Member
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 8 
Quote:
Suggest your flow to be incompressible, take look at this files (numbered by order of calling in program): 1) OpenFOAM1.6/src/finiteVolume/finiteVolume/fvc/fvcDdt.C, function ddtPhiCorr(rA, U, phi), lines 106125 2) OpenFOAM1.6/src/finiteVolume/finiteVolume/ddtSchemes/EulerDdtScheme/EulerDdtScheme.C, procedure EulerDdtScheme<Type>::fvcDdtPhiCorr(rA, U, phiAbs). lines 372  402 3) OpenFOAM1.6/src/finiteVolume/finiteVolume/ddtSchemes/ddtScheme/ddtScheme.C, procedure ddtScheme<Type>::fvcDdtPhiCoeff(U, phi), lines 138233 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 

January 12, 2010, 02:51 

#11 
Senior Member

Thank you Matvej for such detailed explanations! Now this point is clear for me.
All the best!
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben FranzJosefStr. 18 A  8700 Leoben Österreich / Austria Tel.: +43 3842  402  3125 http://smmp.unileoben.ac.at 

January 29, 2010, 05:44 

#12 
Senior Member
Claus Meister
Join Date: Aug 2009
Location: Wiesbaden, Germany
Posts: 241
Rep Power: 8 
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 

January 29, 2010, 06:34 

#13 
Senior Member
Kathrin Kissling
Join Date: Mar 2009
Location: Besigheim, Germany
Posts: 134
Rep Power: 8 
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 

February 5, 2010, 03:15 
help

#14 
Member
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 6 
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 

February 5, 2010, 08:30 

#15 
Senior Member

Mohsen,
first try to read at least User and Programmer guides, that would help you to avoid such questions. Good luck!
__________________
Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Advanced Process Simulation of Solidification and Melting" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben FranzJosefStr. 18 A  8700 Leoben Österreich / Austria Tel.: +43 3842  402  3125 http://smmp.unileoben.ac.at 

March 20, 2010, 16:27 

#16  
Member
YS
Join Date: Jan 2010
Posts: 66
Rep Power: 7 
Quote:
Hi, mkraposhin I was wondering where can we find the mathematical derivation of this treatment or justification? Thanks a lot! 

April 18, 2010, 08:46 
help

#17 
Member
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 6 
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 

April 18, 2010, 08:53 
help

#18 
Member
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 6 
hello again
when compiling a code I get the following message : mohsen@mohsenlaptop:~/OpenFOAM/OpenFOAM1.6/src/transportModels$ ./Allwmake + wmake libso incompressible '/home/mohsen/OpenFOAM/OpenFOAM1.6/lib/linuxGccDPOpt/libincompressibleTransportModels.so' is up to date. + wmake libso interfaceProperties '/home/mohsen/OpenFOAM/OpenFOAM1.6/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@mohsenlaptop:~/OpenFOAM/OpenFOAM1.6/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 

June 16, 2010, 12:44 

#19 
Senior Member
Join Date: Apr 2010
Posts: 151
Rep Power: 7 
A little suggestion: sometimes people forget to run "wclean" before "wmake", provoking the error you had.


December 14, 2011, 22:39 
Why grad(U)().T() and not grad(U).T()

#20 
Member
Rui Vizinho de Oliveira
Join Date: Sep 2011
Posts: 31
Rep Power: 5 
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 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
OpenFoam programming  prapanj  OpenFOAM  10  March 18, 2010 08:23 
Programming in OpenFOAM  vinu  OpenFOAM  2  July 11, 2009 10:16 
two questions about udf programming  Vincent  FLUENT  1  October 5, 2008 00:24 
new CFD Programming Forum  Thinker  Main CFD Forum  14  November 19, 2002 17:03 
Programming in C  Tony  Main CFD Forum  5  March 7, 2002 13:40 