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

Overflow in hypersonic flow simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 21, 2014, 21:33
Exclamation Overflow in hypersonic flow simulation
  #1
Member
 
Join Date: May 2013
Posts: 40
Rep Power: 4
badboyz31 is on a distinguished road
Hello there,

Once again, I'm using CFX to do a simulation of a conical waverider in Mach 6 flow. I generated the model myself and meshed it using ICEM CFD. The meshing type I used was all Quad. The atmospheric condition is set to ISA at 20 km.

In CFX, the fluid domain is set to ideal gas, reference pressure is 0, total energy.

I'm using 4 boundary conditions, the supersonic inlet (velocity, static pressure, static temperature), supersonic outlet, farfield (subsonic, opening pressure, opening temperature), and finally no slip wall for the waverider.

The advection scheme is upwind and physical timescale is set to 1E-05. However, "Overflow" came out right after the 1st iteration. Maybe I'm doing a mistake. I didn't use double precision though.

Thanks in advance. I'll post any screenshot if anybody needs it.
badboyz31 is offline   Reply With Quote

Old   February 22, 2014, 05:34
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
No need for the images just yet. This is a FAQ, but I have not written the FAQ for it yet.

You need to improve the numerical stability. The answer (as I just posted on another thread), is improve mesh quality, double precision numerics, smaller time step and/or better initial condition. Some combination of those will fix it (providing the flow is physically possible).

In your case I bet your time step size is too big. Probably other problems as well, but I bet this is a key one.
ghorrocks is offline   Reply With Quote

Old   February 22, 2014, 18:41
Default
  #3
Member
 
Join Date: May 2013
Posts: 40
Rep Power: 4
badboyz31 is on a distinguished road
Ah, I did forgot to set a smaller timescale and to use double precision. Thanks, I'll wait patiently for the longer iteration as long as it converges. By the way, is it possible to change timestep during the iteration ?
badboyz31 is offline   Reply With Quote

Old   February 22, 2014, 19:29
Default
  #4
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 291
Rep Power: 6
RicochetJ is on a distinguished road
I think you can change the timestep during a run by using the tool "Edit Run In Progress".

If you're doing a transient simulation use adaptive timestepping, with a minimum and maximum timestep of 1e-10 and 1e+10 s respectively. The solver will determine which timestep is the best for the given convergence criteria.
RicochetJ is offline   Reply With Quote

Old   February 26, 2014, 07:08
Default
  #5
Member
 
Join Date: May 2013
Posts: 40
Rep Power: 4
badboyz31 is on a distinguished road
Okay, smaller timescale and double precision did let the program to iterate longer, however another problem arise. The maximum mach number notice keep rising with each iteration until it reached about 1e11 before giving error : fatal bounds, absolute pressure in default domain.

Anything else that might be wrong ? I did a check on my mesh and I think it should be tight enough.
badboyz31 is offline   Reply With Quote

Old   February 26, 2014, 07:40
Default
  #6
siw
Senior Member
 
Join Date: Jul 2009
Posts: 446
Rep Power: 14
siw will become famous soon enough
Does switching on the High Speed Numerics option make any difference? See CFX-Pre User's Guide > 20. Solver Control > 20.6. Advanced Options Tab.
siw is offline   Reply With Quote

Old   February 26, 2014, 17:45
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Another trick to try for supersonic flow is to use Local Time Stepping, set to about 5.0. This can be useful. But make sure you change back to physical time stepping for the final run to convergence - you can do this with Change Run In Progress.
ghorrocks is offline   Reply With Quote

Old   February 26, 2014, 19:41
Default
  #8
Member
 
Join Date: May 2013
Posts: 40
Rep Power: 4
badboyz31 is on a distinguished road
Okay will try these tips. Thanks for your info guys.
badboyz31 is offline   Reply With Quote

Old   February 26, 2014, 20:42
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
I did a check on my mesh and I think it should be tight enough.
Comments like that make me smile. Did you do a sensitivity check against an accuracy tolerance you are happy with? Or did you just look at it and it looks kinda fine? The first is useful, the second is useless.

And also be aware that as you refine the mesh the numerical instability increases. So convergence gets harder to achieve. So a good idea can be to run a coarse mesh to convergence (which should be quick and easy) and use that as an initial condition for a finer mesh simulation.
ghorrocks is offline   Reply With Quote

Old   February 27, 2014, 08:24
Default
  #10
Member
 
Join Date: May 2013
Posts: 40
Rep Power: 4
badboyz31 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Comments like that make me smile. Did you do a sensitivity check against an accuracy tolerance you are happy with? Or did you just look at it and it looks kinda fine? The first is useful, the second is useless.

And also be aware that as you refine the mesh the numerical instability increases. So convergence gets harder to achieve. So a good idea can be to run a coarse mesh to convergence (which should be quick and easy) and use that as an initial condition for a finer mesh simulation.

Ah yes, I'm a fool. I did just look at it and I thought that I should create mesh as fine as possible to achieve better convergence. Thanks for the reminder though, I'm completely noob when it comes to sensitivity check.
badboyz31 is offline   Reply With Quote

Old   March 7, 2014, 12:18
Default Error: Floating point error: overflow Error Object: ().
  #11
New Member
 
Join Date: Apr 2013
Posts: 3
Rep Power: 4
Benkoussas is on a distinguished road
I need help, I am trying to simulate a muliphasique flow (non newotonien fluid / air) in a pipe 2D, my non newotonien fluid follows the law of Herschelle bulkley, and as initial condition, I have a profile unsteady pressure, I started the calculation with a time step 10 ^ -5, it converges after 230 iterations then displays me the following message: Error: Floating point error: overflow Error Object: ().
I don't know exactly where is the problem??
Benkoussas is offline   Reply With Quote

Old   March 7, 2014, 12:21
Default Error: Floating point error: overflow Error Object: ().
  #12
New Member
 
Join Date: Apr 2013
Posts: 3
Rep Power: 4
Benkoussas is on a distinguished road
my boundary conditions:

inlet: pressure inlet (profile unsteady pressure udf)
outlet: pressure outlet
axis and wall
Benkoussas is offline   Reply With Quote

Old   March 7, 2014, 12:34
Default Error: Floating point error: overflow Error Object: ()
  #13
New Member
 
Join Date: Apr 2013
Posts: 3
Rep Power: 4
Benkoussas is on a distinguished road
if someone can help me here is my e-mail:

h.benkoussas@gmail.com

I Thank You in advance
Benkoussas is offline   Reply With Quote

Old   March 8, 2014, 05:33
Default
  #14
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

But you shoudl expect numerical instability with a non-newtonian model in a multiphase simulation. This means you should expect to need a high quality mesh, small time steps, double precision numerics and a good initial condition.
ghorrocks is offline   Reply With Quote

Reply

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
Domain format problem on airfoil flow simulation andrenonaka CFX 6 December 4, 2014 04:57
Hypersonic Flow simulation using Fluent beanlee999 FLUENT 15 October 14, 2014 00:30
problems in synthetic jet flow simulation jackxu FLUENT 0 December 2, 2012 10:12
Problem, solidworks flow simulation castaway FloEFD, FloWorks & FloTHERM 3 September 11, 2012 12:44
Review: Reversed flow CRT FLUENT 0 July 20, 2012 13:03


All times are GMT -4. The time now is 00:36.