CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Programming & Development (http://www.cfd-online.com/Forums/openfoam-programming-development/)
-   -   viscoelastic flow with free surface (http://www.cfd-online.com/Forums/openfoam-programming-development/86662-viscoelastic-flow-free-surface.html)

 chnrdu March 29, 2011 12:03

viscoelastic flow with free surface

1 Attachment(s)
I am interested in the viscoelastic flow with free surface.

Thanks Favero, who gives me a way to solve it.

But I have tried the numerical algorithm, and have not get the right solution.

I combined the interFoam and viscoelasticFluidFoam, and using the Giesekus constitutive model for viscoelastic flow.

The attachment is my combined source. I think the critical part is the constitutive correction of tauP ( in the source, it is tau_), and divTau(U)

the tauP correction is
fvSymmTensorMatrix tauEqn
(
etaP()*lambda()*fvm::ddt(tau_)
+ etaP()*lambda()*fvm::div(phi(), tau_)
==
sqr(etaP())*twoD
+ etaP()*lambda()*twoSymm(C)
- lambda()*(alpha())*(tau_ & tau_)
- etaP()*fvm::Sp(scalar(1), tau_)
)

where the etaP, lambda and alpha is respectively the combined two phase value with respectively gamma.

the divTau(U) is

fvc::div(tau_)
- fvm::laplacian(etaPf(), U)
+ fvm::laplacian( (etaPf()+etaSf()), U)

Thank you very much!

Martin

 chnrdu March 30, 2011 19:08

1 Attachment(s)
When I compute, The tau is divergent at the position circled. It becomes very larger than its vicinity.

How to correct it?

Thank you very much!

-------------------
Martin

 sharonyue January 2, 2013 05:12

Quote:
 Originally Posted by chnrdu (Post 301579) When I compute, The tau is divergent at the position circled. It becomes very larger than its vicinity. How to correct it? Thank you very much! ------------------- Martin
Hi,Martin

Have this problem been handled?

 thejaraju December 11, 2013 03:13

Hi chandru
this is theja from bangalore....
actually i am also working on viscoelasticinterfoam for simulating blow moulding analysis from past one month.....
The current OF which i am working is OF2.2.x. can your share how did you couple the above solver i.e., viscoelasticInterfoam.v2 in the existing OF.

theja

 wyldckat December 25, 2013 14:13

Greetings to all!

@thejaraju:
Quote:
 Originally Posted by thejaraju (Post 465837) The current OF which i am working is OF2.2.x. can your share how did you couple the above solver i.e., viscoelasticInterfoam.v2 in the existing OF.

Best regards,
Bruno

 ovie March 4, 2014 19:10

Viscoelastic Free Surface Flows

2 Attachment(s)
Hi Foamers:

Has anyone been able to reproduce the numerical results for viscoelastic free surface flows reported by Favero et al in their paper: "Viscoelastic fluid analysis in internal and in free surface flows using the software OpenFOAM". I have been working on this for some time now but havent had any success getting the same results.

Let me provide some background to my implementation and workflow.

1.) First, I coupled interFoam with viscoelasticFluidFoam by defining a viscoelasticTwoPhaseMixture class similar to what was done by chnrdu in the first post on this thread.

2.) In the new class, I implemented the correct() function for solving the stress transport equations and divTau() function for coupling momentum equation with viscoelastic stress contribution.

3.) Finally UEqn.H in the viscoelasticInterFoam solver is modified accordingly to include contribution from viscoelastic effects.

My source files are attached.

In the paper there were 4 cases i.e case A - D corresponding to a combination of different values for alpha, lambda and etaP.

For case A, where the relaxation time is 0.03s, my simulations run without any problems. However, I canot reproduce the die-swell phenomenon at the channel exit.

When I increase the relaxation time to 0.3s, the computation runs for a while and then stops as velocity becomes unbounded at the inlet even though Dirichlet conditions were specified. Mules solver fails and gives a floating

So my question is has anyone been able to reproduce these results without any problems? If yes, could please shed some light on how to solve some of the challenges I am dealing with?

Thanks.

compiling viscoelasticMultiphaseMixture

hi everybody,

I'm trying to compile the viscoelasticMultiphaseMixture that Ovie placed here earlier and adding Giesekus constitutive equation to it. When I compiled the code the following error was appeared which I can't solve it:

Code:

```viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C: In constructor ‘Foam::viscoelasticTwoPhaseMixture::viscoelasticTwoPhaseMixture(const volVectorField&, const surfaceScalarField&, const Foam::word&)’: viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:76:41: error: ‘lookup’ was not declared in this scope     phase1Name_(wordList(lookup("phases"))[0] : "phase1"),                                         ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:84:32: error: ‘subDict’ was not declared in this scope             subDict(phase1Name_),                                 ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:142:27: error: ‘found’ was not declared in this scope             found("phases") ? word("alpha" + phase1Name_) : alpha1Name,                           ^ In file included from viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:26:0: viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.H:114:14: warning: ‘Foam::viscoelasticTwoPhaseMixture::viscosityType_’ will be initialized after [-Wreorder]         word viscosityType_;               ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.H:86:27: warning:  ‘Foam::dimensionedScalar Foam::viscoelasticTwoPhaseMixture::etaS1_’ [-Wreorder]         dimensionedScalar etaS1_;                           ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:65:1: warning:  when initialized here [-Wreorder]  Foam::viscoelasticTwoPhaseMixture::viscoelasticTwoPhaseMixture  ^ In file included from viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:26:0: viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.H:120:27: warning: ‘Foam::viscoelasticTwoPhaseMixture::k_’ will be initialized after [-Wreorder]         dimensionedScalar k_;                           ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.H:74:31: warning:  ‘const volVectorField& Foam::viscoelasticTwoPhaseMixture::U_’ [-Wreorder]         const volVectorField& U_;                               ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:65:1: warning:  when initialized here [-Wreorder]  Foam::viscoelasticTwoPhaseMixture::viscoelasticTwoPhaseMixture  ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:197:5: error: no matching function for call to ‘Foam::transportModel::transportModel(const volVectorField&, const surfaceScalarField&)’     )     ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:197:5: note: candidates are: In file included from viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.H:38:0,                 from viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:26: /home/mostafa/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/transportModel/transportModel.H:72:9: note: Foam::transportModel::transportModel()         transportModel         ^ /home/mostafa/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/transportModel/transportModel.H:72:9: note:  candidate expects 0 arguments, 2 provided /home/mostafa/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/transportModel/transportModel.H:57:9: note: Foam::transportModel::transportModel(const Foam::transportModel&)         transportModel(const transportModel&);         ^ /home/mostafa/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/transportModel/transportModel.H:57:9: note:  candidate expects 1 argument, 2 provided viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C: In member function ‘virtual bool Foam::viscoelasticTwoPhaseMixture::read()’: viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:334:49: error: ‘subDict’ was not declared in this scope             nuModel1_().read(subDict(phase1Name_))                                                 ^ viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C:382:1: warning: control reaches end of non-void function [-Wreturn-type]  }  ^ make: *** [Make/linux64GccDPOpt/viscoelasticTwoPhaseMixture.o] Error 1```
the red bolded lines are referring to:
Code:

```Foam::viscoelasticTwoPhaseMixture::viscoelasticTwoPhaseMixture (     const volVectorField& U,     const surfaceScalarField& phi,     const word& alpha1Name ) :     transportModel(U, phi),     phase1Name_(found("phases") ? wordList(lookup("phases"))[0] : "phase1"),     phase2Name_(found("phases") ? wordList(lookup("phases"))[1] : "phase2"),     nuModel1_     (         viscosityModel::New         (             "nu1",             subDict(phase1Name_),             U,             phi         )     ),     nuModel2_     (         viscosityModel::New         (             "nu2",             subDict(phase2Name_),             U,             phi         )     ), . . .```
and I don't know how can I define for it catching the viscoelastic properties from the user.
Actually the structure of transportPropertis file is changed and I should define the way that code can reach the data in the new structure.

anybody is here knows what should I do?

Regards,
Mostafa

 wyldckat February 6, 2015 09:53

Quote:
 Originally Posted by adambarfi (Post 530708) anybody is here knows what should I do?
Quick question: Which OpenFOAM version are you using?

Quote:
 Originally Posted by wyldckat (Post 530729) Quick question: Which OpenFOAM version are you using?
hi Bruno,

OF-231!

Is it important which version I'm using?

 wyldckat February 7, 2015 07:23

1 Attachment(s)
Hi Mostafa,
Quote:
 Originally Posted by adambarfi (Post 530735) OF-231! Is it important which version I'm using?
Because from the test I just made, the source code seems to have been designed to be compiled with OpenFOAM 2.2.2 or 2.2.x.
Apparently for this particular code, the new additions and evolutions in OpenFOAM 2.3.x were too many and the code needs to be adapted.

In specific, the "transportModel" class in OpenFOAM 2.3 does not inherit from "IOdictionary", therefore it does not have a dictionary ready to be used, which is the main reason for the current problems you're having.

The changes I needed to do were as follows:
Code:

```diff -Nur viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C viscoelasticTwoPhaseMixture23/viscoelasticTwoPhaseMixture.C --- viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.C    2014-03-04 21:27:47.000000000 +0000 +++ viscoelasticTwoPhaseMixture23/viscoelasticTwoPhaseMixture.C    2015-02-07 11:19:25.269367298 +0000 @@ -69,7 +69,18 @@     const word& alpha1Name  )  : -    transportModel(U, phi), +    IOdictionary +    ( +        IOobject +        ( +            "transportProperties", +            U.time().constant(), +            U.db(), +            IOobject::MUST_READ_IF_MODIFIED, +            IOobject::NO_WRITE +        ) +    ), +    twoPhaseMixture(U.mesh(), *this),       phase1Name_(found("phases") ? wordList(lookup("phases"))[0] : "phase1"),     phase2Name_(found("phases") ? wordList(lookup("phases"))[1] : "phase2"), diff -Nur viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.H viscoelasticTwoPhaseMixture23/viscoelasticTwoPhaseMixture.H --- viscoelasticTwoPhaseMixture/viscoelasticTwoPhaseMixture.H    2014-02-26 18:58:47.000000000 +0000 +++ viscoelasticTwoPhaseMixture23/viscoelasticTwoPhaseMixture.H    2015-02-07 11:15:46.281375065 +0000 @@ -35,10 +35,11 @@  #ifndef viscoelasticTwoPhaseMixture_H  #define viscoelasticTwoPhaseMixture_H   -#include "incompressible/transportModel/transportModel.H" -#include "incompressible/viscosityModels/viscosityModel/viscosityModel.H"  #include "dimensionedScalar.H"  #include "volFields.H" +#include "incompressible/transportModel/transportModel.H" +#include "incompressible/viscosityModels/viscosityModel/viscosityModel.H" +#include "twoPhaseMixture.H"  #include "fvm.H"  #include "fvc.H"  #include "fvMatrices.H" @@ -55,7 +56,9 @@    class viscoelasticTwoPhaseMixture  : -    public transportModel +    public IOdictionary, +    public transportModel, +    public twoPhaseMixture  {  protected:```
The source code is attached. I based my code changes on the class "src/transportModels/incompressible/incompressibleTwoPhaseMixture".

Best regards,
Bruno

Thanks Bruno,

I will try it, and thanks again for the comprehensive explanation.

Regards,
Mostafa

 vigges March 17, 2015 07:41

Hi Bruno,

I am trying to compile ovie's viscoelasticInterFoam with your viscoelasticTwoPhaseMixture, however, some errors occur during the compilation process.

When compiling the viscoelasticTwoPhaseMixture model from within the solver directory by running "wmake libso viscoelasticTwoPhaseMixture", I got following error:
Code:

```In file included from viscoelasticTwoPhaseMixture.C:26:0: viscoelasticTwoPhaseMixture.H: In member function ‘virtual Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::viscoelasticTwo viscoelasticTwoPhaseMixture.H:205:10: warning: no return statement in function returning non-void [-Wreturn-type]         {}           ^ viscoelasticTwoPhaseMixture.H: In constructor ‘Foam::viscoelasticTwoPhaseMixture::viscoelasticTwoPhaseMixture(const volVectorField&, const surfaceScalarFiel viscoelasticTwoPhaseMixture.H:116:14: warning: ‘Foam::viscoelasticTwoPhaseMixture::viscosityType_’ will be initialized after [-Wreorder]         word viscosityType_;               ^ viscoelasticTwoPhaseMixture.H:88:27: warning:  ‘Foam::dimensionedScalar Foam::viscoelasticTwoPhaseMixture::etaS1_’ [-Wreorder]         dimensionedScalar etaS1_;                           ^ viscoelasticTwoPhaseMixture.C:65:1: warning:  when initialized here [-Wreorder]  Foam::viscoelasticTwoPhaseMixture::viscoelasticTwoPhaseMixture  ^ In file included from viscoelasticTwoPhaseMixture.C:26:0: viscoelasticTwoPhaseMixture.H:122:27: warning: ‘Foam::viscoelasticTwoPhaseMixture::k_’ will be initialized after [-Wreorder]         dimensionedScalar k_;                           ^ viscoelasticTwoPhaseMixture.H:76:31: warning:  ‘const volVectorField& Foam::viscoelasticTwoPhaseMixture::U_’ [-Wreorder]         const volVectorField& U_;                               ^ viscoelasticTwoPhaseMixture.C:65:1: warning:  when initialized here [-Wreorder]  Foam::viscoelasticTwoPhaseMixture::viscoelasticTwoPhaseMixture  ^ /usr/lib64/gcc/x86_64-suse-linux/4.8/../../../../x86_64-suse-linux/bin/ld: cannot find -ltwoPhaseInterfaceProperties collect2: error: ld returned 1 exit status```
I was able to resolve that problem by adjusting the options file within the model's Make directory, though, I'm still getting the above stated warning messages.
Code:

```diff -Nur viscoelasticTwoPhaseMixture/Make/OLDoptions viscoelasticTwoPhaseMixture/Make/options --- viscoelasticTwoPhaseMixture/Make/OLDoptions 2015-02-07 12:18:15.000000000 +0100 +++ viscoelasticTwoPhaseMixture/Make/options    2015-03-17 12:21:07.383486910 +0100 @@ -7,7 +7,7 @@     -I\$(LIB_SRC)/finiteVolume/lnInclude    LIB_LIBS = \ -    -ltwoPhaseInterfaceProperties \ +    -linterfaceProperties \     -lincompressibleTransportModels \     -lincompressibleTurbulenceModel \     -lincompressibleRASModels \```
After adjusting the solver's option file as follows

Code:

```--- Make/OLDoptions    2015-03-17 12:34:32.901429259 +0100 +++ Make/options        2015-03-17 12:27:47.210504016 +0100 @@ -1,5 +1,7 @@  EXE_INC = \ +    -IviscoelasticTwoPhaseMixture/lnInclude \     -I\$(LIB_SRC)/transportModels \ +    -I\$(LIB_SRC)/transportModels/twoPhaseMixture/lnInclude \     -I\$(LIB_SRC)/transportModels/incompressible/lnInclude \     -I\$(LIB_SRC)/transportModels/interfaceProperties/lnInclude \     -I\$(LIB_SRC)/turbulenceModels/incompressible/turbulenceModel \```
I get following error messages:

Code:

```In file included from viscoelasticInterFoam.C:47:0: viscoelasticTwoPhaseMixture/lnInclude/viscoelasticTwoPhaseMixture.H: In member function ‘virtual Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::viscoelasticTwoPhaseMixture::nu() const’: viscoelasticTwoPhaseMixture/lnInclude/viscoelasticTwoPhaseMixture.H:205:10: warning: no return statement in function returning non-void [-Wreturn-type]         {}           ^ In file included from viscoelasticInterFoam.C:63:0: createFields.H: In function ‘int main(int, char**)’: createFields.H:33:33: error: cannot declare variable ‘twoPhaseProperties’ to be of abstract type ‘Foam::viscoelasticTwoPhaseMixture’     viscoelasticTwoPhaseMixture twoPhaseProperties(U, phi);                                 ^ In file included from viscoelasticInterFoam.C:47:0: viscoelasticTwoPhaseMixture/lnInclude/viscoelasticTwoPhaseMixture.H:57:7: note:  because the following virtual functions are pure within ‘Foam::viscoelasticTwoPhaseMixture’:  class viscoelasticTwoPhaseMixture       ^ In file included from viscoelasticTwoPhaseMixture/lnInclude/viscoelasticTwoPhaseMixture.H:40:0,                 from viscoelasticInterFoam.C:47: /software/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/transportModel/transportModel.H:86:34: note:      virtual Foam::tmp<Foam::Field<double> > Foam::transportModel::nu(Foam::label) const         virtual tmp<scalarField> nu(const label patchi) const = 0;                                   ^ In file included from viscoelasticInterFoam.C:95:0: pEqn.H:12:9: error: ‘ddtPhiCorr’ is not a member of ‘Foam::fvc’       + fvc::ddtPhiCorr(rAU, rho, U, phi)         ^ In file included from viscoelasticInterFoam.C:64:0: /software/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude/readTimeControls.H:38:8: warning: unused variable ‘maxDeltaT’ [-Wunused-variable]  scalar maxDeltaT =```
Do you happen to have an idea how to solve this problem?

Best regards,
Victor

 wyldckat April 4, 2015 17:31

2 Attachment(s)
Greetings Victor,

Well, this was a bit of a mess of a code... I only managed to take care of the building problems, by taking into account how the original OpenFOAM source code evolved. I do not have a test case (nor the time) to test this.

Attached are the updated packages, built to work with OpenFOAM 2.3.1 and 2.3.x.
Make sure you unpack the two packages in the same folder, not one inside the other, before building them.

Best regards,
Bruno

 vigges April 5, 2015 15:23

Bruno,

it's working :) Thank you very much!!! Best easter present this year!! :D

Based on that, I'm now gonna try to implement the multimode model into the existing solver.

 arash.heidarian April 13, 2015 10:31

????

hi fomers
what is gamma in this solver?
does any one have a case which have been solved with this solver(viscointerfoam)?
i would be really thanksfull if anyone answer.
thanks

 Supersale April 15, 2015 23:14

Hi vigges, do you maybe have a test case for this solver?

Hi everybody,

I've compiled the viscoelasticTwoPhaseMixture and the solver succressfully :D, but I have some problems with transportProperties file :(

what should I write next to the transportModel?

I tested the it like below:

Code:

```phases (water air); water { //    transportModel  Newtonian; //    nu              nu [ 0 2 -1 0 0 0 0 ] 1e-06;     rho            rho [ 1 -3 0 0 0 0 0 ] 998.2;     rheology     {                 type FENE-P;                 rho              rho [1 -3 0 0 0 0 0] 998.2;                 etaS            etaS [1 -1 -1 0 0 0 0] 8.9e-04;                 etaP            etaP [1 -1 -1 0 0 0 0] 8.9e-04;                 lambda          lambda [0 0 1 0 0 0 0] 0.04;                 L2              L2 [0 0 0 0 0 0 0] 6.0;   }     CrossPowerLawCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         m              m [ 0 0 1 0 0 0 0 ] 1;         n              n [ 0 0 0 0 0 0 0 ] 0;     }     BirdCarreauCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         k              k [ 0 0 1 0 0 0 0 ] 99.6;         n              n [ 0 0 0 0 0 0 0 ] 0.1003;     } } air { //    transportModel  Newtonian; //    nu              nu [ 0 2 -1 0 0 0 0 ] 1.48e-05;     rho            rho [ 1 -3 0 0 0 0 0 ] 1.225;     rheology     {                 type FENE-P;                 rho              rho [1 -3 0 0 0 0 0] 1.225;                 etaS            etaS [1 -1 -1 0 0 0 0] 1.789e-05;                 etaP            etaP [1 -1 -1 0 0 0 0] 1.789e-05;                 lambda          lambda [0 0 1 0 0 0 0] 1e-5;                 L2              L2 [0 0 0 0 0 0 0] 6.0;   }     CrossPowerLawCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         m              m [ 0 0 1 0 0 0 0 ] 1;         n              n [ 0 0 0 0 0 0 0 ] 0;     }     BirdCarreauCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         k              k [ 0 0 1 0 0 0 0 ] 99.6;         n              n [ 0 0 0 0 0 0 0 ] 0.1003;     } } sigma          sigma [ 1 0 -2 0 0 0 0 ] 0.07;```
but it said that the presence of transportModel is necessary! :confused:

Does anybody know what should I do?

Regards,
Mostafa

Solved! :cool:

the transportProperties should be like this:
Code:

```phases (water air); water {     transportModel  Newtonian;     nu              nu [ 0 2 -1 0 0 0 0 ] 1e-06;     rho            rho [ 1 -3 0 0 0 0 0 ] 998.2;                 rheology        FENE-P;                 viscosityType    "else";                 rho              rho [1 -3 0 0 0 0 0] 998.2;                 etaS            etaS [1 -1 -1 0 0 0 0] 8.9e-04;                 etaP            etaP [1 -1 -1 0 0 0 0] 8.9e-04;                 lambda          lambda [0 0 1 0 0 0 0] 0.04;                 L2              L2 [0 0 0 0 0 0 0] 6.0;                 epsilon                epsilon [0 0 0 0 0 0 0] 0;                 zeta                zetta [0 0 0 0 0 0 0] 0;                 Alpha                Alpha [0 0 0 0 0 0 0] 0;                 mu0                mu0 [1 -1 -1 0 0 0 0] 0;                 muInf                mu0 [1 -1 -1 0 0 0 0] 0;                 a                mu0 [1 -1 -1 0 0 0 0] 0;                 b                mu0 [1 -1 -1 0 0 0 0] 0;                 k                mu0 [1 -1 -1 0 0 0 0] 0; //  }     CrossPowerLawCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         m              m [ 0 0 1 0 0 0 0 ] 1;         n              n [ 0 0 0 0 0 0 0 ] 0;     }     BirdCarreauCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         k              k [ 0 0 1 0 0 0 0 ] 99.6;         n              n [ 0 0 0 0 0 0 0 ] 0.1003;     } } air {     transportModel  Newtonian;     nu              nu [ 0 2 -1 0 0 0 0 ] 1.789e-05;     rho            rho [ 1 -3 0 0 0 0 0 ] 1.225;                 rheology        FENE-P;                 viscosityType    "else";                 rho              rho [1 -3 0 0 0 0 0] 1.225;                 etaS            etaS [1 -1 -1 0 0 0 0] 1.789e-05;                 etaP            etaP [1 -1 -1 0 0 0 0] 1.789e-05;                 lambda          lambda [0 0 1 0 0 0 0] 1e-5;                 L2              L2 [0 0 0 0 0 0 0] 6.0;                 epsilon                epsilon [0 0 0 0 0 0 0] 0;                 zeta                zetta [0 0 0 0 0 0 0] 0;                 Alpha                Alpha [0 0 0 0 0 0 0] 0;                 mu0                mu0 [1 -1 -1 0 0 0 0] 0;                 muInf                mu0 [1 -1 -1 0 0 0 0] 0;                 a                mu0 [1 -1 -1 0 0 0 0] 0;                 b                mu0 [1 -1 -1 0 0 0 0] 0;                 k                mu0 [1 -1 -1 0 0 0 0] 0; //  }     CrossPowerLawCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 1e-06;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         m              m [ 0 0 1 0 0 0 0 ] 1;         n              n [ 0 0 0 0 0 0 0 ] 0;     }     BirdCarreauCoeffs     {         nu0            nu0 [ 0 2 -1 0 0 0 0 ] 0.0142515;         nuInf          nuInf [ 0 2 -1 0 0 0 0 ] 1e-06;         k              k [ 0 0 1 0 0 0 0 ] 99.6;         n              n [ 0 0 0 0 0 0 0 ] 0.1003;     } } sigma          sigma [ 1 0 -2 0 0 0 0 ] 0.07;```
But I still don't know what to do with transportModel??:confused:

 vigges April 22, 2015 16:04

Supersale, I had to turn my attention to single phase viscoelastic flow. So, unfortunately, my efforts regarding the multiphase problem will be somewhat reduced for the time being, but I will get back to this thread when I have something presentable.

 arash.heidarian April 24, 2015 03:26

thanks Mr mahmoudi it was really helpfull....

All times are GMT -4. The time now is 13:01.