[chnrdu]

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)

Please help me to review the source.

Thank you very much!

Martin

[chnrdu]

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]

Originally Posted by chnrdu

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]

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.

thanking you in advance and waiting eagerly for reply

theja

[wyldckat]

Greetings to all!

@thejaraju:

Originally Posted by thejaraju

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.

I'll answer you on your other thread, namely: http://www.cfd-online.com/Forums/ope...ion-error.html

Best regards,
Bruno

[ovie]

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.

[adambarfi]

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:

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:

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]

Originally Posted by adambarfi

anybody is here knows what should I do?

Quick question: Which OpenFOAM version are you using?

[adambarfi]

Originally Posted by wyldckat

Quick question: Which OpenFOAM version are you using?

hi Bruno,

OF-231!

Is it important which version I'm using?

[wyldckat]

Hi Mostafa,

Originally Posted by adambarfi

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:

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

[adambarfi]

Thanks Bruno,

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

Regards,
Mostafa

[vigges]

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:

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.

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

--- 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:

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]

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]

Bruno,

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

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

[arash.heidarian]

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]

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

[adambarfi]

Hi everybody,

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

what should I write next to the transportModel?

I tested the it like below:

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!

Does anybody know what should I do?

Regards,
Mostafa

[adambarfi]

Solved!

the transportProperties should be like this:

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??

[vigges]

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]

thanks Mr mahmoudi it was really helpfull....