
[Sponsors] 
September 30, 2010, 02:17 
uncoupledKinematicParcelFoam Examples

#1 
New Member
Chris Butler
Join Date: Jun 2010
Posts: 21
Rep Power: 8 
Hi all,
I am trying to do some simple Lagrangian particle calculations with OpenFOAM. The actual computation of the particles is relatively simple: One case with solid particles within an incompressible flow One case with massless infinitesimal particles (i.e. stream tracers calculated within OF). I need to do this with respect to both a steady state and unsteady flow field. I have two questions then: 1) Is uncoupledKinematicParcelFoam the right solver for for the the problem at hand? It looks to me like it may not be able to evolve over a changing flow field. 2) How do I setup a case with uncoupledKinematicParcelFoam? Everything seems to go to hell when I need a temperature field for my fluid. Cheers, Chris Butler 

October 1, 2010, 02:59 

#2 
Senior Member
matej forman
Join Date: Mar 2009
Location: Brno, Czech Republic
Posts: 104
Rep Power: 9 
Hi,
the nature of all ways how to compute the particles in OpenFoam is transient. uncoupledKinematicParcelFoam can be used for computation of a flow field already computed. The solver reads this field and does numerical integration of lagrangian equations on it using kinematicParcel class. So it's a kind of aposteriori method. You can use it for changing flowfield, but you need appropriate frequency of time steps stored. The steadystate issue  if you have a steady state flow you may run a transient computation with large time steps for long enough time for particle to pass through the domain. The temperature issue  the kinematicParcel cloud is defining isothermal particles. you would need to use thermalParcel or if you want reactions, reactingParcel class. They are all described in $FOAM/src/lagrangian/intermediate. It looks very messy and complicated but it's not that bad. For your application you can use several approaches: (1) adopt the uncoupledKinematicParcelFoam to thermalParcel (2) use some solver which computes the particles together with the flowfield (especially if the particles are exchanging heat with the surrounding, yoy shoud run the particles together with the flow anyway) like reactingParcelFoam without the reactions. (3) use spray class. good luck matej 

October 3, 2010, 21:03 

#3  
New Member
Chris Butler
Join Date: Jun 2010
Posts: 21
Rep Power: 8 
Quote:
It seems that I had a more fundamental problem than I thought. Now my C++ is pretty poor, however, I think the problem is that the basicKinematicCloud constructor (inherited from KinematicCloud) presumes a compressible field (i.e. requires volumetric fields for rho and mu). This is also reflected in createFields.H for the solver. For incompressible solvers I think that the passiveParticle library is what needs to be used. Chris Butler 

October 4, 2010, 04:05 

#4 
Senior Member
matej forman
Join Date: Mar 2009
Location: Brno, Czech Republic
Posts: 104
Rep Power: 9 
Hi Chris,
You are right you need density and viscosity of the fluid to calculate the drag. But you may easily create these fields in the start directory and use this approach. Or you may use passive scalar as well. There are several ways. It is true that the passive scalar seems to be more easy to understand the code. good luck matej 

October 6, 2010, 00:26 
passiveParticleCloud Help!

#5 
New Member
Chris Butler
Join Date: Jun 2010
Posts: 21
Rep Power: 8 
Hi all,
Wondering if anyone has had success with passiveParticleFoam. I am am trying (as a first stage) to reimplement uncoupledKinematicParcelFoam for a incompressible solver. I am having trouble finding how to 'evolve' the particles. I think the function is: Foam::Cloud::move() However, my C++ is rudimentary and I don't quite understand the follow error: passiveParticleParcelFoam.C:61:21: error: no matching function for call to ‘Foam:assiveParticleCloud::move()’ Any help would be much appreciated. Chris Butler 

October 6, 2010, 03:15 

#6 
Senior Member
matej forman
Join Date: Mar 2009
Location: Brno, Czech Republic
Posts: 104
Rep Power: 9 
Hi Chris,
the error clearly saiz what's wrong. There is no function move() for passiveParticleCloud defined. You should have the definition in the definition of class passiveParticleCloud. The compiler cannot find it. Now the thing with the compressibility.... The computation of uncoupledKinematicParcelFoam is not compressible at all. Look where the mu a rho is used in the code. You will find that it's used only for the particles the fluid flow is still incompressible. the mu and rho is there only for the implementation reasons as when you extend the kinematic to thermal cloud, you have rho and mu in the field anyway so you do not need to have extra overloading of the clouds. good luck with you c++ matej 

October 6, 2010, 22:56 

#7 
New Member
Chris Butler
Join Date: Jun 2010
Posts: 21
Rep Power: 8 
Hi Matej,
I figured out my confusion. Because the Cloud class was templat'ed it did not inherit Foam::Cloud::move(). I think that you are right that the existing uncoupledKinematicParcelFoam will be easier to work with. It looks like passiveParticleCloud is not implemented. All i have to do is trick KinematicCloud into thinking I have a density field. Chris Butler 

August 18, 2015, 12:37 
icoUncoupledKinematicParcelFoam TwoWay Coupling

#8 
New Member
matin
Join Date: Nov 2014
Posts: 3
Rep Power: 3 
Hi everyone,
I'm trying to use icoUncoupledKinematicParcelFoam solver for the TwoWay coupling by turning the "Coupled" option "On" in the KinematicCloudProperties directory. I ran a case, having fluid flow and particles, and noticed that the flow field does not change and it seems turning the "Couple" option On or Off does not affect the simulation and it solves for OneWay coupling. I have read that this solver is suitable for the precalculated velocity field and that the particles do not affect the fluid field, but why they have defined such option in the KinematicCloudProperties directory to couple and decoupled the simulation ? I also know that there are other solvers like DPMFoam and MPPICFoam which consider twoway coupling, but I want to know whether I can use icoUncoupledKinematicParcelFoam solver for twoway coupling or not. I really appreciate if anyone could give me some information about their experience using this solver, Thanks, Matin 

August 19, 2015, 03:48 

#9 
Senior Member
matej forman
Join Date: Mar 2009
Location: Brno, Czech Republic
Posts: 104
Rep Power: 9 
Hi,
as the name of the solver says it is uncoupled, so trying to use it for coupling is nogo even from the grammatical point of view. The best way to find out what your solver can or cannot do is to read the description in the source of the solver. In your case try: less $FOAM_SOLVERS/lagrangian/icoUncoupledKinematicParcelFoam/icoUncoupledKinematicParcelFoam.C and read the description, where you will learn that this solver is reading the velocity fields in previously calculated and stored in appropriate time directories and evolves (integrates the lagrangian equation for the particle) in this velocity field. So no coupling whatsoever. happy foaming 

August 19, 2015, 21:00 

#10 
New Member
matin
Join Date: Nov 2014
Posts: 3
Rep Power: 3 
Matej,
Thank you so much for your prompt response. 

July 8, 2016, 13:46 

#11  
New Member
Darko Radenkovic
Join Date: Oct 2015
Posts: 23
Rep Power: 2 
Quote:
How to set up pseudo  transient approach? Due to integration of Newton's law of motion, time step has to be small and Courant number has to be less than 1. Also if soft sphere model is used, with large time step, computation time is going to be very high. How to overcome this problem? Regards, Darko 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
VOF examples needed, please!  Freeman  FLUENT  5  February 3, 2011 17:28 
Examples of microfluids  A Siddiqui  Main CFD Forum  3  November 8, 2005 04:03 
SIMPLE, SIMPLER Examples  Maciej Matyka  Main CFD Forum  9  November 3, 2003 06:11 
examples of simulation on room ventilation?  lei  FLUENT  1  June 20, 2003 22:38 
Wanted: Examples of Deforming Meshes  Greg Perkins  Main CFD Forum  3  June 25, 2001 08:10 