# Low Machnumber combustion LES

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 28, 2005, 07:08 Hi All, I want to us OpenFo #1 Michael Oevermann (Oevermann) Guest   Posts: n/a Hi All, I want to us OpenFoam for LES combustion in the low Mach-number regime. There are two questions to start with: 1) which is the most appropriate solver in Foam to start with? Is it PISO or should we use a different scheme? 2) I am also interested to solve the equations in the zero Mach-number limit. In that case the energy equation reduces to a divergence constraint for the velocity leading to a pressure poisson equation. This will lead to a projection method type of scheme. Is there a fast solver for the poisson equation implemented? If yes, what kind of solver is it (AMG, Krylov subspace?). How difficult is it to set up and solve a poisson problem with the unstructured grid in foam? Best regards Michael ------------------------------------------------------- Dr. Michael Oevermann Technische Universität Berlin Institut für Energietechnik Fasanenstr. 89, 10623 Berlin, Germany Phone: +49 (0) 30 314 22452 Fax: +49 (0) 30 314 22157 mailto: michael.oevermann@tu-berlin.de -------------------------------------------------------

 January 28, 2005, 07:31 1) Xoodles - sounds like exac #2 Hrvoje Jasak (Hjasak) Guest   Posts: n/a 1) Xoodles - sounds like exactly what you need. It is a pressure-based compressible formulation using PISO. 2) Compressible PISO also solves a pressure equation - for the incompressibility limit you just lose the convection and the ddt terms. In this formulation, the varying compressibility just changes the nature of the pressure equation from hyperbolic (compressible) to elliptic (incompressible) and the solver can deal with both. Foam contains both ICCG (Incomplete Cholesky preconditioned Conjugate Gradient) and AMG (Algebraic Multigrid) solvers. Both are excellent and the performance for elliptic problems is really not an issue. Solving a Poisson equation is very easy - study the tutorials, because I suspect you'll spend more time learning how to use foam than actually solving the Poisson problem. Enjoy, Hrv

 January 31, 2005, 13:39 Hrvoje, thanks for the in #3 Michael Oevermann (Oevermann) Guest   Posts: n/a Hrvoje, thanks for the information! Do you know if the AMG and ICCG are running on parallel machines? What is the speedup? Michael

 January 31, 2005, 17:45 Can I do a Rolls-Royce trick #4 Hrvoje Jasak (Hjasak) Guest   Posts: n/a Can I do a Rolls-Royce trick :-) and say the speed-up is "sufficient"? Foam is massively parallel and has been used up to 256 CPU-s (maybe more), with decent scaling results. The problem with concrete numbers is that it is very difficult to pick a representative case and a machine that will give proper data: if a case is too small it does not have enough work per node and if it is too big it does not fit onto a single CPU. I have done a test on a big Silicon Graphics (in a domain decomposition mode) and got speed up of about 11 on 16 CPU on a non-dedicated machine - there was other jobs running, the bus was loaded etc. so this is not the mest you can get. As a general rule, you don't have to worry about parallel scaling - it is appropriate for the purpose and foam does parallelism well (that's how all the LES work is done). As a guideline on the solver choice, ICCG scales better in parallel than AMG. AMG tends to talk a lot on the top-level (it does not reconstruct the top-level matrix on one node). This can be improved (it's been sitting on my to-do list for ages) but I don't see the priority. AMG is bets used whan ICCG tends to use a lot of iterations, either due to the mesh quality or tight solution tolerances. Enjoy, Hrv

 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 wuyu FLUENT 7 October 21, 2015 13:18 popi CFX 7 July 11, 2007 18:40 Jessy FLUENT 1 June 19, 2007 10:59 George Main CFD Forum 0 September 7, 2006 14:41 prasat Main CFD Forum 1 June 16, 2003 13:17

All times are GMT -4. The time now is 23:19.

 Contact Us - CFD Online - Top