# Courant number and implicit treatment

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

 January 17, 2008, 18:52 Hi there, was just wonderin #1 Member   Patrick Bourdin Join Date: Mar 2009 Posts: 40 Rep Power: 8 Hi there, was just wondering: in icoFoam, the momentum equations are treated implicitly, so why is there a Courant number limitation wrt stability? Fully implicit methods should not suffer from that, or am I missing anything here? Cheers. Patrick

 January 17, 2008, 19:10 hi, courant number limit is #2 Senior Member   Stephan Gerber Join Date: Mar 2009 Location: Germany Posts: 118 Rep Power: 8 hi, courant number limit is a stability limit for explicit methods. but still using courant numbers above one with an implicit method is stable but information gets transported faster as it should. i am not sure if everybody here does agree but this were my first thoughts... br stephan

 January 18, 2008, 07:47 Hello, you have also to not #3 Member   Rosario Russo Join Date: Mar 2009 Location: Trieste, Italy Posts: 56 Rep Power: 8 Hello, you have also to notice that in icofoam the algorithm considers weak non linear coupling in momentum equations with respect to pressure velocity coupling: this is why momentum equations are solved only once per timestep. The assumption is true only at small Courant numbers. So you have to be sure to have Courant numbers less than 0.5 at least. Rosario

 January 18, 2008, 11:16 hi rosario, why do you thin #4 Senior Member   Stephan Gerber Join Date: Mar 2009 Location: Germany Posts: 118 Rep Power: 8 hi rosario, why do you think that icoFoam solves "weakly coupled" equations - it looks like the standard piso which always needs at least two corrector stages?! br stephan

 January 18, 2008, 12:24 Hi, pressure and velocity a #5 Member   Rosario Russo Join Date: Mar 2009 Location: Trieste, Italy Posts: 56 Rep Power: 8 Hi, pressure and velocity are strongly coupled and so PISO needs a correction loop, but the momentum equations are considered "frozen" even if velocity and pressure are corrected in the loop, so they are not solved again for the current time step. This means that the advection terms in the momentum equations are considered not much coupled among themselves. This is true only at small Courant numbers. Rosario.

 January 18, 2008, 17:37 hi rosario, i dont see the #6 Senior Member   Stephan Gerber Join Date: Mar 2009 Location: Germany Posts: 118 Rep Power: 8 hi rosario, i dont see the point: piso solves one predictor and two correctors for the velocity: the momentum equation is solved three time and thats exactly what issa recommends in his paper (his error analysis convinced at least me and himself) on the other hand:is there any incomp. transient single phase solver which does different in foam, if yes which one? i guess we can stop at the point that we simply disagree... br stephan

 January 19, 2008, 07:23 Sorry probably I was unclear, #7 Member   Rosario Russo Join Date: Mar 2009 Location: Trieste, Italy Posts: 56 Rep Power: 8 Sorry probably I was unclear, I'm trying to explain it better. Anyway please correct me something is not correct. icofoam PISO algorithm: 1) momentum equations are used in an implicit way to find a predictor value for velocity. The old value is used for pressure. 2) Using new velocity values, momentum and mass conservation, a Poisson equation is constructed. 3) The Poisson equation is solved. New p values and new velocities (satisfying now continuity) are found. step 2) and 3) are repeated. In my opinion the point with Courant is that in 2) and 3) (pressure correction loop), the momentum equations are used to compute a new velocity according to the new p, and velocities are found explicitly not implicitly, like at point 1. This makes necessary to assume weak coupling in non linear momentum terms and so small Co. Am i wrong?

 January 19, 2008, 16:29 Dear Rosario, The segregate #8 Member   Patricio Bohorquez Join Date: Mar 2009 Location: Jaén, Spain Posts: 94 Rep Power: 8 Dear Rosario, The segregated solution technique implemented in FOAM corresponds to successive substitution. Therefore there is no guarantee a converged solution can be reached (Jasak H, 2006). This fact is independent of the Courant number. For instance, you can think in a steady flow: If you knew the solution of the problem and used it as the first guess of the numerical solver with a large Courant number (Co>1), the solution would preserve equal to the initial guess. Moreover, if you introduced a small perturbation over this solution, "perturbation amplitudes would decrease" as time went on if the background flow was stable and the numerical solver was implicit, independent of the Courant number - this stability criteria is obtained from a linear stability analysis and therefore it should be carefully applied to non-linear problems. On the other hand, perturbation amplitudes would increase if an explicit scheme was employed with Co>1. However, the case described above is not general. For a transient problem, the solution is changing from one to next time step. In the successive substitution approach, the coupling terms will be evaluated from the currently available solution and lagged. If the solution changes abruptly in time, successive substitution does not guarantee convergence - this fact is not related to the explicit/implicit character of the numerical scheme. If you got stability problems, a small Courant number and relaxing the equations would help to stabilize the numerical solution. Best wishes, Patricio Jasak H (2006) Numerical Solution Algorithms for Compressible Flows. Lecture Notes: University of Zagreb, Croatia Tobi and abtinansari like this.

 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 CH Main CFD Forum 1 March 14, 2007 08:51 CFX Novice CFX 1 July 26, 2006 13:40 andy Main CFD Forum 5 June 9, 2006 11:03 cfd worker CFX 1 February 8, 2006 21:15 raintung FLUENT 3 May 7, 2003 06:03

All times are GMT -4. The time now is 18:41.