
[Sponsors] 
December 2, 2011, 10:22 
scalarTransportFoam

#1 
New Member
Join Date: Oct 2011
Posts: 14
Rep Power: 6 
Hello Folks,
Iam new to OpenFoam and there are so many things I have not yet figured out. I would like to model the transport equation for different species. I have inlet flows with different concentrations and would like to see how the concentrations spread in my volume. I understand I could use scalarTransportFoam a couple of times, i.e. for each concentration, but there should be a way to solve all the transport equations at once? I understand modelling chemical reactions in OF is difficult. Especially in fluids. Why cant the scalar transport equation just be extended by the sourceterm and then solved? Iam sure, the answers to my questions are straightforward to most of you. I would appreciate any answer. Thanks. 

December 2, 2011, 12:53 

#2 
Senior Member
David Gaden
Join Date: Apr 2009
Location: Winnipeg, Canada
Posts: 426
Rep Power: 14 
Exactly my area of research.
SOLVING MULTIPLE TRANSPORT EQUATIONS AT ONCE Often it is conventional to solve the governing equations simultaneously, e.g. in systems of ODEs. But continuum mechanics have PDEs as governing equations, and these are not conventionally solved simultaneously because it's much harder. Even for incompressible laminar flow, we solve continuity first, then momentum (pressure) second. The problem comes in trying to "couple" these two solution methods. It took many decades of research before some efficient algorithms were developed  SIMPLE and PISO. If you want to solve the PDE equations *simultaneously*, these solvers are now available. Not in OpenFOAM2.0.x, but look in OpenFOAMextend1.6.x. They have what's known as a "blockcoupled matrix solver". The one in OpenFOAMextend is very powerful, in that it can be used to solve any kind of block coupled matrix: pointimplicit, full coupled, with scalars, vectors, tensors, etc.. There are two main kinds of blockcoulped matrices. A "pointimplicit", where the coupling effects between variables are only local to each cell, and "fullcoupled", where the coupling effects between variables extend throughout the entire control volume. The fullcoupled solver is very taxing on computer memory. So if you would be able to use a 2 million element mesh with a conventional solver, a fullcoupled solver would only allow you to use say 200,000 elements for the same memory. If you want to solve the flow field, you need a fullycoupled solver. But if you only want to solve chemical reactions, you can probably get by with a pointimplicit solver. SOLVING REACTIONS There are three options I see: 1. Fully segregated: i) solve the flow, ii) transport the species, iii) solve the reactions. All of these are done separately. The timestep is limited by the Nyquist criterion. This is how rhoReactingFoam works, for example. 2. Pointimplicit: i) solve the flow, ii) the transport and react the species. The second step is your pointimplicit solver. It combines reactions and transport, but it requires a static flow field. The timestep is not limited by the Nyquist criterion, but the question is: how much will the reactions affect the flow field? How safe is the larger timestep? For combustion, I'd think it wouldn't differ too much from option 1. 3. Fullycoupled. Solve the flow, reactions, and species transport all together. This would have a huge memory footprint, which probably would scale exponentially with the number of species involved. But this would be totally independent of the Nyquist criterion. I hope that helps!
__________________
~~~ Follow me on twitter @DavidGaden 

February 6, 2012, 21:21 

#3 
Senior Member
David Gaden
Join Date: Apr 2009
Location: Winnipeg, Canada
Posts: 426
Rep Power: 14 
Not Nyquist. I mean Courant number. Writing my thesis now and I realized I've been using the wrong term all along.
__________________
~~~ Follow me on twitter @DavidGaden 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
ScalarTransportFoam for RTD calculations  santoo_cfd  OpenFOAM Running, Solving & CFD  34  May 22, 2014 10:20 
Problem with scalarTransportFoam illistrated using pitzDaily tutorial  mlawson  OpenFOAM  2  January 18, 2011 14:39 
Units in scalartransportfoam  Frithjof  OpenFOAM  1  January 5, 2011 11:41 
ScalarTransportFoam  skabilan  OpenFOAM Running, Solving & CFD  3  April 15, 2010 12:28 
flux seems not conserved in my modified scalarTransportFoam  danielr  OpenFOAM Running, Solving & CFD  3  October 5, 2009 16:05 