
[Sponsors] 
October 6, 2010, 15:43 

#2 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 22 
Hmm, I think actually only variation of viscosity by volume fraction is taken into account, not by nonlinear viscosity laws. But it could be implemented.
Best.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 Int. 7032 Colectora Ruta Nac. 168 / Paraje El Pozo (3000) Santa Fe  Argentina. http://www.cimec.org.ar 

October 8, 2010, 20:03 

#4 
Senior Member
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 22 
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 nonnewtonian 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: 543424511594 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: 727
Rep Power: 20 
Nonnewtonian 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 runtime 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: 452
Rep Power: 22 
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 ); Best.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 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: 1,265
Blog Entries: 1
Rep Power: 23 
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: 727
Rep Power: 20 
Yes Santiago, you are probably right. In 1.5 there was rasInterFoam and lesInterFoam.
There is already a nearcomplete example of nonNewtonian 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: 452
Rep Power: 22 
Hi, from CrossPowerLaw.C we have:
Code:
00051 Foam::tmp<Foam::volScalarField> 00052 Foam::viscosityModels::CrossPowerLaw::calcNu() const 00053 { 00054 return (nu0_  nuInf_)/(scalar(1) + pow(m_*strainRate(), n_)) + nuInf_; 00055 }
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D. Research Scientist Research Center for Computational Methods (CIMEC)  CONICET/UNL Tel: 543424511594 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
Posts: 226
Rep Power: 15 
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: 1,265
Blog Entries: 1
Rep Power: 23 
hi again
im still looking for a reference in nonNewtonain 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
Posts: 226
Rep Power: 15 

October 18, 2010, 05:46 
HI

#14 
Senior Member
Join Date: Sep 2010
Posts: 226
Rep Power: 15 
Hi
here are the definitions in constant/transportProperties directory transportModel CrossPowerLaw CrossPowerLawCoeffs { nu0 nu0 [0 2 1 0 0 0 0] 1e06; nuInf nuInf [0 2 1 0 0 0 0] 1e06; m m [0 0 1 0 0 0 0] 1; n n [0 0 0 0 0 0 0] 1; } 

October 18, 2010, 07:54 
HI

#16  
Senior Member
Join Date: Sep 2010
Posts: 226
Rep Power: 15 
Quote:
http://www.cfdonline.com/Forums/ope...itymodel.html 

August 7, 2019, 16:13 
Implemention of NonNewtonian model in Interfoam

#17 
New Member
tooran
Join Date: Nov 2016
Posts: 23
Rep Power: 8 
Hi all,
I am trying to apply nonnewtonian model interfoam. In transport properties, instead of newtonian model I intered HerschelBulkley and HerschelBulkleyCoeffs. After running it shows me erro. The transport properties file is written as below: FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object transportProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // phases (water air); water { transportModel HerschelBulkley; { HerschelBulkleyCoeffs nu0 [ 0 2 1 0 0 0 0 ] 1e+03; tau0 [ 0 2 2 0 0 0 0 ] 0.016; k [ 0 2 1 0 0 0 0 ] 0.02; n [ 0 0 0 0 0 0 0 ] 1; } } air { transportModel HerschelBulkley; { HerschelBulkleyCoeffs nu0 [ 0 2 1 0 0 0 0 ] 1e+03; tau0 [ 0 2 2 0 0 0 0 ] 0.001; k [ 0 2 1 0 0 0 0 ] 0.0023; n [ 0 0 0 0 0 0 0 ] 1; } } sigma 0.07; // ************************************************** *********************** // ************************************************** ************************ I think interfoam solver needs to have rho for both phases as input. But I don't know where I should put rho as input? Could you please help me? Thanks 

August 7, 2019, 16:59 

#18 
New Member
tooran
Join Date: Nov 2016
Posts: 23
Rep Power: 8 
I found my problem the correct form of transport properties should be as below :
******************************** /** C++ **\ =========  \\ / F ield  OpenFOAM: The Open Source CFD Toolbox \\ / O peration  Website: https://openfoam.org \\ / A nd  Version: 6 \\/ M anipulation  \**/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object transportProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // phases (water air); water //concrete { rho rho [1 3 0 0 0 0 0] 2500.0; transportModel HerschelBulkley; HerschelBulkleyCoeffs { nu0 [ 0 2 1 0 0 0 0 ] 1e+03; //[ 0 2 1 0 0 0 0 ] tau0 [ 0 2 2 0 0 0 0 ] 0.016; //[ 0 2 2 0 0 0 0 ] k [ 0 2 1 0 0 0 0 ] 0.02; //[ 0 2 1 0 0 0 0 ] n [ 0 0 0 0 0 0 0 ] 1; //[ 0 0 0 0 0 0 0 ] } } air //lubrication { rho rho [1 3 0 0 0 0 0] 2000.0; transportModel HerschelBulkley; HerschelBulkleyCoeffs { nu0 [ 0 2 1 0 0 0 0 ] 1e+03; tau0 [ 0 2 2 0 0 0 0 ] 0.001; k [ 0 2 1 0 0 0 0 ] 0.0023; n [ 0 0 0 0 0 0 0 ] 1; } } sigma 0.07; // ************************************************** *********************** // ************************************************* 

October 11, 2019, 13:31 

#19 
New Member
Felipe Chagas
Join Date: Feb 2019
Posts: 11
Rep Power: 6 
You tooran,
do you know how to insert nonnewtonian behavior in compressibleInterFoam? It seems that the insertion is different from interFoam... Does anyone know how to do it? Thanks! 

September 16, 2022, 16:15 
interFoam (OFoam v10) + nonnewtonian fluid

#20 
New Member
Márcio Froelich Friedrich
Join Date: Aug 2013
Posts: 1
Rep Power: 0 
Dear Colleagues
I'm trying to set a nonnewtonian fluid simulation with interFoam (air + material from a tailing dam). The solution presented by Tooran with OpenFoam 6.0 does not seem to work with OpenFoam 10. As far as I understand, the choice of a "transportModel" (e.g. HerschelBulkley)  that was made in transportProperties file in version 6.0  is now made in file physicalProperties.water under the name "viscosityModel". The problem is that viscosityModel only accepts 'constant' or 'newtonian'. I did find a interFoam tutorial in which a Maxwell nonnewtonian model is set to the liquid phase, but it is set on momentumTransport.liquid as a laminar model, which is not what I want. I would like to set a RAS turbulent simulation with a nonnewtonian fluid. Any insight is very welcome. Thanks! Last edited by marxioxyz; October 5, 2022 at 16:06. 

Tags 
cross law, interfoam, non newtonian 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
question about turbulence model selection and sensitivity  karananand  Main CFD Forum  1  February 26, 2010 04:41 
Centrifugal Pump and Turbulence Model  Michiel  CFX  12  January 25, 2010 03:20 
Problems bout CFD model of biomass gasification, Downdraft gasifier  wanglong  FLUENT  2  November 25, 2009 23:27 
Reynolds Stress model in CFX vs Fluent  Tim  CFX  1  October 7, 2009 06:19 
Grid resolution for fullscale and down scaled model  gravis  Main CFD Forum  0  October 2, 2009 10:27 