|
[Sponsors] |
March 29, 2011, 12:03 |
viscoelastic flow with free surface
|
#1 |
New Member
|
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 |
|
March 30, 2011, 19:08 |
|
#2 |
New Member
|
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 |
|
January 2, 2013, 04:12 |
|
#3 |
Senior Member
Dongyue Li
Join Date: Jun 2012
Location: Beijing, China
Posts: 844
Rep Power: 18 |
||
December 11, 2013, 02:13 |
|
#4 |
New Member
thejaraju
Join Date: Dec 2010
Posts: 8
Rep Power: 15 |
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 |
|
December 25, 2013, 13:13 |
|
#5 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Greetings to all!
@thejaraju: Quote:
Best regards, Bruno
__________________
|
||
March 4, 2014, 18:10 |
Viscoelastic Free Surface Flows
|
#6 |
Member
Ovie Doro
Join Date: Jul 2009
Posts: 99
Rep Power: 17 |
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. |
|
February 6, 2015, 07:07 |
compiling viscoelasticMultiphaseMixture
|
#7 |
Senior Member
|
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 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 ) ), . . . 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 |
|
February 6, 2015, 09:19 |
|
#9 |
Senior Member
|
||
February 7, 2015, 06:23 |
|
#10 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
Hi Mostafa,
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: Best regards, Bruno
__________________
|
|
February 16, 2015, 05:25 |
|
#11 |
Senior Member
|
Thanks Bruno,
I will try it, and thanks again for the comprehensive explanation. Regards, Mostafa |
|
March 17, 2015, 06:41 |
|
#12 |
Member
Join Date: Oct 2011
Posts: 36
Rep Power: 14 |
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 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$(LIB_SRC)/finiteVolume/lnInclude LIB_LIBS = \ - -ltwoPhaseInterfaceProperties \ + -linterfaceProperties \ -lincompressibleTransportModels \ -lincompressibleTurbulenceModel \ -lincompressibleRASModels \ Code:
--- Make/OLDoptions 2015-03-17 12:34:32.901429259 +0100 +++ Make/options 2015-03-17 12:27:47.210504016 +0100 @@ -1,5 +1,7 @@ EXE_INC = \ + -IviscoelasticTwoPhaseMixture/lnInclude \ -I$(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 \ 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 = Best regards, Victor |
|
April 4, 2015, 17:31 |
|
#13 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,980
Blog Entries: 45
Rep Power: 128 |
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
__________________
|
|
April 5, 2015, 15:23 |
|
#14 |
Member
Join Date: Oct 2011
Posts: 36
Rep Power: 14 |
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. |
|
April 13, 2015, 10:31 |
????
|
#15 |
New Member
arash
Join Date: Jan 2015
Posts: 14
Rep Power: 11 |
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 |
|
April 15, 2015, 23:14 |
|
#16 |
New Member
Sasa Goran
Join Date: Feb 2015
Location: Japan
Posts: 23
Rep Power: 11 |
Hi vigges, do you maybe have a test case for this solver?
|
|
April 22, 2015, 10:38 |
|
#17 |
Senior Member
|
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: 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; Does anybody know what should I do? Regards, Mostafa |
|
April 22, 2015, 14:33 |
|
#18 |
Senior Member
|
Solved!
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; |
|
April 22, 2015, 16:04 |
|
#19 |
Member
Join Date: Oct 2011
Posts: 36
Rep Power: 14 |
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.
|
|
April 24, 2015, 03:26 |
|
#20 |
New Member
arash
Join Date: Jan 2015
Posts: 14
Rep Power: 11 |
thanks Mr mahmoudi it was really helpfull....
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Free surface flow over a bump | qtian | OpenFOAM Running, Solving & CFD | 17 | August 10, 2010 10:15 |
Scaling up a wave energy converter - free surface flow | mark_l | CFX | 3 | February 17, 2010 16:57 |
free surface flow same as FSI??? | Ken | CFX | 1 | February 18, 2008 19:43 |
How to determine delta t for free surface flow | phsieh2005 | Main CFD Forum | 0 | September 14, 2005 11:52 |
incompressible free surface flow past cylinder | vineet | FLUENT | 2 | April 1, 2002 05:56 |