Overflow in hypersonic flow simulation

badboyz31 · February 21, 2014, 20:33

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.

ghorrocks · February 22, 2014, 04:34

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.

badboyz31 · February 22, 2014, 17:41

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 ?

JuPa · February 22, 2014, 18:29

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.

badboyz31 · February 26, 2014, 06:08

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.

siw · February 26, 2014, 06:40

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.

ghorrocks · February 26, 2014, 16:45

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.

badboyz31 · February 26, 2014, 18:41

Okay will try these tips. Thanks for your info guys.

ghorrocks · February 26, 2014, 19:42

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.

badboyz31 · February 27, 2014, 07:24

Quote:

Originally Posted by ghorrocks

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.

Benkoussas · March 7, 2014, 11:18

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 · March 7, 2014, 11:21

my boundary conditions:

inlet: pressure inlet (profile unsteady pressure udf)
outlet: pressure outlet
axis and wall

Benkoussas · March 7, 2014, 11:34

if someone can help me here is my e-mail:

h.benkoussas@gmail.com

I Thank You in advance

ghorrocks · March 8, 2014, 04:33

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.

February 21, 2014, 20:33	Overflow in hypersonic flow simulation	#1
badboyz31 Member Join Date: May 2013 Posts: 45 Rep Power: 12	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.

March 7, 2014, 11:18	Error: Floating point error: overflow Error Object: ().	#11
Benkoussas New Member Join Date: Apr 2013 Posts: 3 Rep Power: 13	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??

March 7, 2014, 11:21	Error: Floating point error: overflow Error Object: ().	#12
Benkoussas New Member Join Date: Apr 2013 Posts: 3 Rep Power: 13	my boundary conditions: inlet: pressure inlet (profile unsteady pressure udf) outlet: pressure outlet axis and wall

March 7, 2014, 11:34	Error: Floating point error: overflow Error Object: ()	#13
Benkoussas New Member Join Date: Apr 2013 Posts: 3 Rep Power: 13	if someone can help me here is my e-mail: h.benkoussas@gmail.com I Thank You in advance

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Hypersonic Flow simulation using Fluent	beanlee999	FLUENT	16	February 5, 2020 20:09
Review: Reversed flow	CRT	FLUENT	1	May 7, 2018 05:36
Domain format problem on airfoil flow simulation	andrenonaka	CFX	14	December 7, 2015 00:42
problems in synthetic jet flow simulation	jackxu	FLUENT	0	December 2, 2012 09:12
Problem, solidworks flow simulation	castaway	FloEFD, FloWorks & FloTHERM	3	September 11, 2012 12:44

February 22, 2014, 04:34		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.

February 22, 2014, 17:41		#3
badboyz31 Member Join Date: May 2013 Posts: 45 Rep Power: 12	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 ?

February 22, 2014, 18:29		#4
JuPa Senior Member Mr CFD Join Date: Jun 2012 Location: Britain Posts: 361 Rep Power: 14	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.

February 26, 2014, 06:08		#5
badboyz31 Member Join Date: May 2013 Posts: 45 Rep Power: 12	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.

February 26, 2014, 06:40		#6
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 733 Rep Power: 25	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.

February 26, 2014, 16:45		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.

February 26, 2014, 18:41		#8
badboyz31 Member Join Date: May 2013 Posts: 45 Rep Power: 12	Okay will try these tips. Thanks for your info guys.

March 8, 2014, 04:33		#14
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	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.