# Compressible solver for low Mach

 Register Blogs Members List Search Today's Posts Mark Forums Read

 January 26, 2013, 04:45 Compressible solver for low Mach #1 New Member   Lipo Wang Join Date: Dec 2012 Posts: 14 Rep Power: 6 Dear all, If anybody has the experience in using the compressible solver for very low Mach (thus almost incompressible) cases? Is it possible? If yes, in principle the calculation can be much speeded up because we dont not need to solve the Poission eq for pressure. If no, where is the main problem? Many thanks for your suggestion!

January 26, 2013, 06:32
#2
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 3,350
Rep Power: 37
Quote:
 Originally Posted by nickna Dear all, If anybody has the experience in using the compressible solver for very low Mach (thus almost incompressible) cases? Is it possible? If yes, in principle the calculation can be much speeded up because we dont not need to solve the Poission eq for pressure. If no, where is the main problem? Many thanks for your suggestion!
Hi,
generally, the low-Mach solver is quite different from the standard compressible solver due to the stiff problem (high velocity magnitude of sound waves compared to convective waves).
The method to get a well-conditioned problem often introduces an expansion arounf the M=0 state and consequently an elliptic equation. You can see many textbook, e.g. http://books.google.it/books/about/C...4C&redir_esc=y

 January 26, 2013, 07:16 #3 Senior Member   cfdnewbie Join Date: Mar 2010 Posts: 557 Rep Power: 13 But in general, yes, it is possible to use a compressible solver in a low Mach number setting, but the timestep will become very small (or the accuracy very low)...

January 26, 2013, 07:37
#4
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 3,350
Rep Power: 37
Quote:
 Originally Posted by cfdnewbie But in general, yes, it is possible to use a compressible solver in a low Mach number setting, but the timestep will become very small (or the accuracy very low)...
I agree, even small perturbations in the numerical solution of the density equation will be amplified in the pressure ... I had experience that the Mach number to work on should be not lesser than 0.1 - 0.05 ...

 January 26, 2013, 22:40 #5 Senior Member   Martin Hegedus Join Date: Feb 2011 Posts: 479 Rep Power: 12 Yes, it is possible with Mach number preconditioning. But, you lose time accuracy.

 January 27, 2013, 05:23 #6 Super Moderator     Praveen. C Join Date: Mar 2009 Location: Bangalore Posts: 259 Blog Entries: 6 Rep Power: 11 There is a preconditioned Roe scheme in which the dissipation is modified to yield correct scheme in the low mach limit. There is also an AUSM version which performs well in low mach limit but I dont recall its precise name now. These are all consistent flux functions which lead to time accurate schemes. However they require very small time step for stability and implicit schemes are necessary. E.g., SU2 code has a preconditioned Roe scheme. See for example http://www.sciencedirect.com/science...45793003000781 which has a very nice asymptotic analysis of upwind schemes in low mach limit. In the following paper, they show that above preconditioned scheme if used in explicit version requires time step of order mach^2 which is too restrictive and hence an implicit scheme is needed for efficiency http://link.springer.com/article/10....0009-0?LI=true A different approach is advocated in this paper http://www.sciencedirect.com/science...21999108000429 where the reconstruction process is modified to get well behaved schemes in low mach limit. A similar approach is given here http://elib.dlr.de/76675/1/ICCFD7-2204_paper.pdf __________________ http://twitter.com/cfdlab

 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 sankarv OpenFOAM Running, Solving & CFD 17 December 3, 2014 20:41 sankarv OpenFOAM 0 April 4, 2010 18:06 diaw Main CFD Forum 104 February 16, 2006 06:44 Endee FLUENT 8 September 7, 2005 16:16 yeo FLUENT 4 March 7, 2003 08:08

All times are GMT -4. The time now is 15:44.