CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

acoustic courant number 999

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   August 30, 2015, 20:57
Default acoustic courant number 999
  #1
rae
New Member
 
Join Date: May 2011
Posts: 20
Rep Power: 8
rae is on a distinguished road
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.
rae is offline   Reply With Quote

Old   August 30, 2015, 22:02
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,837
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   August 31, 2015, 00:13
Default
  #3
New Member
 
Costin Ruja
Join Date: Mar 2010
Location: Bucharest
Posts: 22
Rep Power: 8
costinruja is on a distinguished road
Send a message via Yahoo to costinruja
@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 ?
costinruja is offline   Reply With Quote

Old   August 31, 2015, 00:21
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,837
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   August 31, 2015, 00:26
Default
  #5
New Member
 
Costin Ruja
Join Date: Mar 2010
Location: Bucharest
Posts: 22
Rep Power: 8
costinruja is on a distinguished road
Send a message via Yahoo to costinruja
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
costinruja is offline   Reply With Quote

Old   August 31, 2015, 01:39
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,837
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   August 31, 2015, 05:46
Default Thanks glen,
  #7
rae
New Member
 
Join Date: May 2011
Posts: 20
Rep Power: 8
rae is on a distinguished road
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.
rae is offline   Reply With Quote

Old   November 2, 2016, 10:27
Default
  #8
New Member
 
skywalker
Join Date: Oct 2016
Posts: 6
Rep Power: 2
M.Meki is on a distinguished road
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
M.Meki is offline   Reply With Quote

Old   November 2, 2016, 18:12
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,837
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your formula for CFL is incorrect. It should be delta_t = delta_x/(abs(flow velocity)+sonic speed).

Have you checked your flow velocities?
ghorrocks is offline   Reply With Quote

Old   November 2, 2016, 18:24
Default
  #10
New Member
 
skywalker
Join Date: Oct 2016
Posts: 6
Rep Power: 2
M.Meki is on a distinguished road
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.
M.Meki is offline   Reply With Quote

Old   November 2, 2016, 18:29
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,837
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
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.
ghorrocks is offline   Reply With Quote

Old   November 4, 2016, 19:25
Default
  #12
New Member
 
skywalker
Join Date: Oct 2016
Posts: 6
Rep Power: 2
M.Meki is on a distinguished road
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.
M.Meki is offline   Reply With Quote

Old   November 5, 2016, 05:36
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,837
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
You mentioned this is a 2D simulation. What is the thickness of your mesh in the z dimension?
ghorrocks is offline   Reply With Quote

Reply

Tags
acoustic courant number, convection, p-mass

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
decomposePar -allRegions stru OpenFOAM Pre-Processing 2 August 25, 2015 03:58
Sudden jump in Courant number NJG OpenFOAM Running, Solving & CFD 7 May 15, 2014 13:52
RMS Courant Number vs MAX Courant Number zoozoozoo Main CFD Forum 3 June 12, 2012 13:44
LES near wall model & courant number kasim CFX 5 March 16, 2008 19:23
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58


All times are GMT -4. The time now is 23:56.