# nonNewton Model for interFoam

 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 6, 2010, 04:07 nonNewton Model for interFoam #1 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,195 Blog Entries: 1 Rep Power: 16 hi dear friends is non Newtonian viscosity (for example cross law ) applicable in interFoam solver?

 October 6, 2010, 15:43 #2 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 16 Hmm, I think actually only variation of viscosity by volume fraction is taken into account, not by non-linear viscosity laws. But it could be implemented. Best. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 October 7, 2010, 00:49 #3 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,195 Blog Entries: 1 Rep Power: 16 could you explain more !!!!!!!

 October 8, 2010, 20:03 #4 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 16 Nima, in UEqn.H there some lines defining the momentum equation for interFoam, basically it has same terms of usual NS equations for newtonian incompressible fluid plus the term due spatial variation of viscosity fvc::grad(U) & fvc::grad(muEff) and term due surface tension fvc::interpolate(interface.sigmaK())*fvc::snGrad(a lpha1) Treatment of spatial variation of rho depends on what version of FOAM are you using, but your most important point is to add the non newtonian terms. I'm not an expert in that topic, maybe you can post how the non-newtonian momentum looks like, so it could be possible to write it in FOAM language. Regards. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 October 10, 2010, 18:36 #5 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 13 Non-newtonian viscosity is supported by interFoam just like most of the other incompressible solvers. The constitutive model for fluid viscosity is hiding inside the "twoPaseMixture" model, which is updated inside the turbulence model. At its base, the twoPhaseMixture just combines two run-time selectable viscosity models which could be any of those defined in Foam.

 October 10, 2010, 19:06 #6 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 16 Aha, as Eugene said, some lines before there are these ones, Code: 00001 surfaceScalarField muEff 00002 ( 00003 "muEff", 00004 twoPhaseProperties.muf() 00005 + fvc::interpolate(rho*turbulence->nut()) 00006 ); so effects of nonlinearity are taken into account in muEff and fvc::grad(U) & fvc::grad(muEff) term. This is true after solvers unification in 1.6 I think, because in 1.5 interFoam was only for laminar cases, Am I right? Best. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 October 11, 2010, 03:03 #7 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,195 Blog Entries: 1 Rep Power: 16 hi buddies first: as i know the difference between linear or non linear fluid is in the relation between starin and stress so we should consider the non linearity just for viscose term in momentum Equation and it is considered in interFoam , so no more change is needed, am i right? second : where can i find appropriate coefficient for nonNewton fluid, it seems interFoam formula implementation is some how different from typical formulation

 October 11, 2010, 05:54 #8 Senior Member   Eugene de Villiers Join Date: Mar 2009 Posts: 725 Rep Power: 13 Yes Santiago, you are probably right. In 1.5 there was rasInterFoam and lesInterFoam. There is already a near-complete example of non-Newtonian fluid use in the interFoam tutorials. You just need to change the "transportModel" entry in phase1 or phase2 (or both) to match that you need. Unfortunately, the examples do not detail all the different viscosity models, so you might have to dig into the code to find out which coefficients need to be specified.

 October 11, 2010, 16:03 #9 Senior Member     Santiago Marquez Damian Join Date: Aug 2009 Location: Santa Fe, Santa Fe, Argentina Posts: 430 Rep Power: 16 Hi, from CrossPowerLaw.C we have: Code: 00051 Foam::tmp 00052 Foam::viscosityModels::CrossPowerLaw::calcNu() const 00053 { 00054 return (nu0_ - nuInf_)/(scalar(1) + pow(m_*strainRate(), n_)) + nuInf_; 00055 } this is Cross Power Law means for OpenFOAM, values of constant can be changed in ./constant/ransportProperties dictionary. __________________ Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC) - CONICET/UNL Tel: 54-342-4511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe - Argentina. http://www.cimec.org.ar

 October 18, 2010, 05:04 Hi #10 Senior Member   Join Date: Sep 2010 Location: France Posts: 223 Rep Power: 9 Hi guys, how one can use two differnet viscosityModels in the same solver, and how to call the two viscosities from their models, lets say: transportModel1 PowerLaw, tranportModel2 Crosspowerlaw How is that can be done? i don't need to use turbulence, i need something direct like icoFoam, but i'll define my transportModels in the dictionary. Help please?

 October 18, 2010, 05:19 #11 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,195 Blog Entries: 1 Rep Power: 16 hi again im still looking for a reference in non-Newtonain fluid in openFoam, does any body know from where i can find appropriate value for transport model?

October 18, 2010, 05:22
hi
#12
Senior Member

Join Date: Sep 2010
Location: France
Posts: 223
Rep Power: 9
hi if you are looking for the viscosity, it is under fluid.nu() in the non-Newtonian fluid.

Quote:
 Originally Posted by nimasam hi again im still looking for a reference in non-Newtonain fluid in openFoam, does any body know from where i can find appropriate value for transport model?

 October 18, 2010, 05:39 #13 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,195 Blog Entries: 1 Rep Power: 16 thanks T.D but i look for appropriate values FOR EXAMPLE for crosslaw fluid in transportModels subdict in constant directory !!!!!!!!

 October 18, 2010, 05:46 HI #14 Senior Member   Join Date: Sep 2010 Location: France Posts: 223 Rep Power: 9 Hi here are the definitions in constant/transportProperties directory transportModel CrossPowerLaw 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] 1; }

 October 18, 2010, 07:06 #15 Senior Member   Nima Samkhaniani Join Date: Sep 2009 Location: Tehran, Iran Posts: 1,195 Blog Entries: 1 Rep Power: 16 hi T.D thanks again but what fluid do you define ? my problem is here, i dont know where i can find these values for different material ?

October 18, 2010, 07:54
HI
#16
Senior Member

Join Date: Sep 2010
Location: France
Posts: 223
Rep Power: 9
Quote:
 Originally Posted by nimasam hi T.D thanks again but what fluid do you define ? my problem is here, i dont know where i can find these values for different material ?
Hi i think you can find the answer her:
Questions about Cross-Arrhenius and Cross-WLF viscosity model

 Tags cross law, interfoam, non newtonian

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post karananand Main CFD Forum 1 February 26, 2010 05:41 Michiel CFX 12 January 25, 2010 04:20 wanglong FLUENT 2 November 26, 2009 00:27 Tim CFX 1 October 7, 2009 06:19 gravis Main CFD Forum 0 October 2, 2009 10:27

All times are GMT -4. The time now is 09:06.