# acoustic courant number 999

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

 August 30, 2015, 20:57 acoustic courant number 999 #1 New Member   Join Date: May 2011 Posts: 21 Rep Power: 9 Can anyone suggest why acoustic courant number is off scale (>999) in my convection study from start, because I suspect I might then avoid solver crash (overflow at timestep 630 for this run). Other strange feature is P-Mass solver fails about half the time despite showing reasonable rms residuals on hydrodynamic equations. Background: Mesh side lengths are from 0.5mm to 100mm in 15m by 42m domain. Thermal energy source is 140kW/m^3 in 2m^3 volume. Timesteps are 0.01s. Transient analysis domain starts from 0m/s at STP. Transient information prior to crash: Flow velocity throughout domain is convectively driven and less than 12m/s. RMS courant number is 8 (max 77). Temperature maximum is 550C. Mach number maximum is 0.018. Pressure is between -300Pa and 250Pa. Tried: Smaller timesteps -- changes nothing.

 August 30, 2015, 22:02 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,214 Rep Power: 110 The "acoustic Courant Number" is known as the CFL number by most people: https://en.wikipedia.org/wiki/Couran...Lewy_condition It is off the scale as it includes the acoustic velocity of your gas. Assuming you are air at near room temperature the acoustic velocity is about 340m/s, so for your 0.5mm mesh you will need time steps about 1.5e-6 s to get a CFL = 1 approximately. So your 0.01s time steps are off the scale, and reducing them a little bit and they will still be off the scale. If CFL is important in your simulation you have a long way to go. But CFL criterion may not be important to your flow. I would recommend using adaptive time steps, homing in on 3-5 coeff loops per iteration. Make sure the max and min time step size is wide enough you never hit them. Then the solver will find its own time step size.

 August 31, 2015, 00:13 #3 New Member   Costin Ruja Join Date: Mar 2010 Location: Bucharest Posts: 22 Rep Power: 9 @Glenn Sorry to intrude, but at the start of a transient run, the solver manager reports 2 Courant measures, rms Courant and acoustic Courant. What is the difference between them ?

 August 31, 2015, 00:21 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,214 Rep Power: 110 No problem. The forum is here to ask questions so you are welcome to ask. The RMS Courant number is the RMS of the Courant number over the simulation. The acoustic Courant number is actually the Courant-Freidrichs-Lewy (CFL) number which is applicable for compressible flows as it also includes the acoustic velocity.

 August 31, 2015, 00:26 #5 New Member   Costin Ruja Join Date: Mar 2010 Location: Bucharest Posts: 22 Rep Power: 9 I can conclude from this that to be able to accurately predict waves (eg. acoustics and blast/shockwave moving front) I have to keep the acoustic courant close to 1.Is this a valid statement ? Regards, Costin

 August 31, 2015, 01:39 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,214 Rep Power: 110 Yes, for this type of flow you will have a limiting CFL of around 1. But I strongly recommend you do a sensitivity study to objectively determine what you require as it is problem dependent. Also using adaptive time stepping to let the solver take care of it (home in on 3-5 coeff loops) is also a really good way of doing it. umair64 likes this.

 August 31, 2015, 05:46 Thanks glen, #7 New Member   Join Date: May 2011 Posts: 21 Rep Power: 9 Sound waves are unimportant to me (and the solver issue if I understand correctly). I imagined something needed to approach the acoustic velocity for the CFL to be 1 (yet alone 999) but your explanation rightly shows the solver knows better than to take anything for granted. I think I may need to start another thread asking about the reason and criticality of the regular P-Mass equation Failures reported by the Solver.

 November 2, 2016, 10:27 #8 New Member   skywalker Join Date: Oct 2016 Posts: 6 Rep Power: 3 I am studying water hammer in sudden closure of valve in CFX. in my 2-d mesh, the pipe length is 10 m, with 200 parts i.e delta x=0.05m sonic speed is 1483 m/s My question is: I chose a time step of 3.3715 e-5 s to obtain a CFL=1. [for CFL=1, delta_t= delta_x/sonic speed]. However, the rms acoustic courant number reports 745.83 and the max is 999.99. I don't know how this makes sense. Is the solver using other dimensions other than the element size in x direction ? please help thank you

 November 2, 2016, 18:12 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,214 Rep Power: 110 Your formula for CFL is incorrect. It should be delta_t = delta_x/(abs(flow velocity)+sonic speed). Have you checked your flow velocities?

 November 2, 2016, 18:24 #10 New Member   skywalker Join Date: Oct 2016 Posts: 6 Rep Power: 3 Thank you so much for your reply. Well, the initial average velocity across the cross section is 0.383889 m/s which is incomparable to the sonic speed. An extra note: I did a steady state run to obtain the initial flow conditions with a static pressure at inlet (44.66 m water) and a mass flow rate which would give me the above average velocity. I used SST instead of K-e for turbulence because K-e gave me steep velocity changes in the velocity profile between the log layer and the viscous layer. SST worked better and gave me almost the same profile as when I did it on Fluent with K-e and enhanced wall treatment. -> For the transient part of the simulation, I used the same value of pressure at inlet (but with an opening instead of inlet) to allow reverse flow. For the outlet : I tried -a wall, 0 velocity and 0 flow rate. Not sure which would work better actually.

 November 2, 2016, 18:29 #11 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,214 Rep Power: 110 No, you need to look at the simulation results in CFD-Post. You cannot take the average flow rate. Very high Courant numbers like this can be the sign of impending divergence as the velocity field is going bezerk and high velocity flows are whizzing around all over the place. You need to look at the results to see if the flow is realistic or not. M.Meki likes this.

 November 4, 2016, 19:25 #12 New Member   skywalker Join Date: Oct 2016 Posts: 6 Rep Power: 3 I monitored sonic speed, courant number, velocity_u at x = 9.5 m. mid pipe axis . 1-sonic speed: constant at 1483 m/s 2-Courant number starts at around 0.0003 and the decreases to zero then rises again. this value (0.0003) makes sense because the max velocity is around 0.4 and the time step is 3.7e-5 and delta x is 0.05. These values give a courant number of about 3e-4. 3- velocity starts off at U_max and then decrease to zero then rises again. All while the solver reports an Acoustic courant number of 999.99 max.

 November 5, 2016, 05:36 #13 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 14,214 Rep Power: 110 You mentioned this is a 2D simulation. What is the thickness of your mesh in the z dimension?

 Tags acoustic courant number, convection, p-mass

 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 stru OpenFOAM Pre-Processing 2 August 25, 2015 03:58 NJG OpenFOAM Running, Solving & CFD 7 May 15, 2014 13:52 zoozoozoo Main CFD Forum 3 June 12, 2012 13:44 kasim CFX 5 March 16, 2008 19:23 msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58

All times are GMT -4. The time now is 14:13.