|
[Sponsors] |
February 12, 2024, 12:20 |
Openfoam 10/11 - Non-Newtonian Fluid setup
|
#1 |
New Member
Nidal
Join Date: Nov 2018
Posts: 17
Rep Power: 8 |
Hi everyone,
I am struggling to setup a non-newtonian fluid within multiphaseInterFoam. It was straightforward before Openfoam 10 was released, were it was setup within transportProperties. This new method where the non-newtonian model is setup within momentum transport is too confusing. Can someone please help me figure it out. I found a tutorial implementing a non-newtonian fluid within pimpleFoam. But that also makes no sense as the viscosity model is set to "constant" Here is what I have, it managed to run but I am not sure if the crossPowerLaw is applied. MomentumTransport: Code:
simulationType laminar; laminar { model generalisedNewtonian; viscosityModel CrossPowerLaw; CrossPowerLawCoeffs { nu0 [0 2 -1 0 0 0 0] 1-05; nuInf [0 2 -1 0 0 0 0] 1E-12; m [0 0 1 0 0 0 0] 1.00E-03; n [0 0 0 0 0 0 0] 0.7; } } Code:
viscosityModel constant; rho 1000; m 1.00E-03; n 0.7; nu 1E-05; nuInf 1E-12; Code:
PIMPLE: Operating solver in transient mode with 6 outer correctors Reading field p_rgh Reading field U Reading/calculating face flux field phi Selecting viscosity model Newtonian Selecting viscosity model Newtonian Selecting viscosity model constant Selecting turbulence model type laminar Selecting laminar stress model generalisedNewtonian Selecting generalised Newtonian model CrossPowerLaw Reading g Reading hRef Calculating field g.h No MRF models present No fvModels present No fvConstraints present |
|
October 1, 2024, 10:11 |
|
#2 | |
Member
Michael Sukham
Join Date: Mar 2020
Location: India
Posts: 85
Rep Power: 6 |
Quote:
|
||
October 12, 2024, 11:10 |
|
#3 |
Member
Michael Sukham
Join Date: Mar 2020
Location: India
Posts: 85
Rep Power: 6 |
Ok. I think I got it. I have to momentumTransport.water and put the thixotropic model. Although I have to give entries for constant viscosity in physicalProperties. A bit confused here
|
|
October 13, 2024, 13:03 |
|
#4 |
New Member
Wesley T.
Join Date: Apr 2009
Posts: 28
Rep Power: 17 |
Edited to add: a tutorial with a non-Newtonian fluid can be found in the OpenFOAM-12/tutorials/incompressibleVoF/climbingRod. I believe it is also in the same location for OF-10 and OF-11, but I have not confirmed this.
The setup for non-Newtonian fluids were not obvious to me, but after some work and finding the above tutorial, I now have some simulations running with non-Newtonian fluid models. The file structure I ended up using when I was trying to simulate coextusion of 2 food materials looks like this: . ├── 0 │ ├── alpha.ExtrudateA │ ├── p_rgh │ └── U ├── BasicCoExPipe.unv ├── constant │ ├── g │ ├── momentumTransport │ ├── momentumTransport.ExtrudateA │ ├── momentumTransport.ExtrudateB │ ├── phaseProperties │ ├── physicalProperties.ExtrudateA │ ├── physicalProperties.ExtrudateB │ └── polyMesh │ ├── boundary │ ├── faces │ ├── neighbour │ ├── owner │ └── points ├── system │ ├── controlDict │ ├── fvSchemes │ └── fvSolution As you mentioned, there needs to be a value for nu in the physicalProperties, but my testing shows that what that value is does not matter to the result if there is a momentumTransport file defining the non-newtonian fluid properties. Information in my physicalProperties.ExtrudateA is shown below: Code:
FoamFile { format ascii; class dictionary; location "constant"; object physicalProperties.ExtrudateA; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // viscosityModel constant; nu 1.64e-3; rho 1250; Code:
FoamFile { format ascii; class dictionary; location "constant"; object momentumTransport.ExtrudateA; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // simulationType laminar; laminar { model generalisedNewtonian; viscosityModel powerLaw; nuMax 1000000; nuMin 0.1; k 3000; n 0.4; } I have not been able to get non-Newtonian fluids working for the incompressibleMultiphaseVoF solver yet. That solver seems to use the information from the physicalProperties files, despite having the same non-Newtonian properties as above in the momentumTransport files. I hope this information is helpful. If my answer is not clear enough, please let me know and I will try to correct any gaps in the details that may be helpful to you. Wesley Last edited by Wesley; October 13, 2024 at 13:11. Reason: Added a reference to a tutorial using a non-Newtonian fluid model |
|
October 13, 2024, 13:08 |
|
#5 |
Member
Michael Sukham
Join Date: Mar 2020
Location: India
Posts: 85
Rep Power: 6 |
Yes. For me, I have the following
. ├── 0 │** ├── U │** ├── alpha.water.orig │** ├── lambda.water.orig │** ├── lambdaThixotropic:lambda.water │** └── p_rgh ├── Allclean ├── Allrun ├── constant │** ├── g │** ├── momentumTransport │** ├── momentumTransport.air │** ├── momentumTransport.water │** ├── phaseProperties │** ├── physicalProperties.air │** └── physicalProperties.water └── system ├── blockMeshDict ├── controlDict ├── fvSchemes ├── fvSolution └── setFieldsDict I am using incompressibleVoF (interFoam) and checked with damBreak case, the non-newtonian behavior is captured well. Thanks! I havent tried multiphaseVoF (multiphaseEulerFoam ??) |
|
October 19, 2024, 11:08 |
|
#6 | |
New Member
Wesley T.
Join Date: Apr 2009
Posts: 28
Rep Power: 17 |
Quote:
If you try one of the multiphase solvers and get it to work, can you share file structure or files? I recently installed OpenFOAM 9 as a docker image so I can run multiphase with powerLaw fluids. There is something I am not finding or understanding for how to run this with multiphase using non-Newtonian fluids in OpenFOAM 10/11/12. If I get a multiphase non-Newtonian simulation running in OpenFOAM 12 (the version I currently use for other simulations), I will share it. Thank you, Wesley |
||
Tags |
multiphaseinterfoam, non-newtonian, openfoam10 |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Map of the OpenFOAM Forum - Understanding where to post your questions! | wyldckat | OpenFOAM | 10 | September 2, 2021 06:29 |
OpenFOAM v3.0.1 Training, London, Houston, Berlin, Jan-Mar 2016 | cfd.direct | OpenFOAM Announcements from Other Sources | 0 | January 5, 2016 04:18 |
OpenFOAM Training, London, Chicago, Munich, Sep-Oct 2015 | cfd.direct | OpenFOAM Announcements from Other Sources | 2 | August 31, 2015 14:36 |
Overflow Error in Multiphase Modelling with Two Continuous Fluids | ashtonJ | CFX | 6 | August 11, 2014 15:32 |
Terrible Mistake In Fluid Dynamics History | Abhi | Main CFD Forum | 12 | July 8, 2002 10:11 |