CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Convergent-Divergent Nozzle Divergence

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 27, 2017, 18:26
Default Convergent-Divergent Nozzle Residuals diverge rapidly
  #1
New Member
 
Hüseyin Emre
Join Date: Mar 2017
Location: Istanbul
Posts: 8
Rep Power: 7
aeronautics is on a distinguished road
Hi all !
I have a basic problem about CD nozzle. I would like to analyze the flow inside and behind of the nozzle in 2D. To do that, firstly, I started my analysis to examine only flow inside the nozzle without adding any ambience behind the nozzle. I chose this way due to simplicity. Residuals (continuity, x-velocity, y-velocity and energy) converged below 1e-7 except y-velocity which converged slightly below 1e-4. On the other hand, when I ran my calculation with the same parameters after adding a rectangular-shaped flow domain just behind the nozzle, it went to diverge after several converging iterations, suddenly, with such a warning on console :

"# Divergence detected in AMG solver: Coupled -> Decreasing coarsening group size!
# Divergence detected in AMG solver: Coupled -> Increasing relaxation sweeps!
# You may try the enhanced divergence recovery with (rpsetvar 'amg/protective-enhanced? #t)"

I could see these warnings on console as well: "Divergence detected - temporarily reducing Courant number to X
and trying again..." and "time step reduced in xxx cells due to excessive temperature change". I am really confused about what I am doing wrong.

Setup;
General: Density-Based
Model: Energy-On, Inviscid
Material: Air-Ideal Gas
Boundary Conditions: Pressure-Inlet, Outlet, Wall
(Inlet Total Gauge Pressure: 4166484 Pa, Initial Gauge Pressure:4157919 Pa, Operating Conditions: 0 Pa, Outlet Total Gauge Pressure:101325 Pa)

I will appreciate if I get some help

Emre

Last edited by aeronautics; August 29, 2017 at 19:40.
aeronautics is offline   Reply With Quote

Old   August 29, 2017, 17:24
Default
  #2
New Member
 
Hüseyin Emre
Join Date: Mar 2017
Location: Istanbul
Posts: 8
Rep Power: 7
aeronautics is on a distinguished road
I've tried to decrease Courant number to 0.1 and ran the calculation about over 1000 iterations then I've increased to Courant number to 1 and ran again. Also have tried to decrease Positivity Rate Limit yet nothing has changed. Afterwards I've ran the calculation after Flux type has been changed to AUSM which provides better solutions in case of occuring shock but it didn't work as well. There already should not any shock waves as a result of my analytical calculations with isentropic & quasi-1D flow and calorically perfect gas assumptions. Any help ?

Last edited by aeronautics; August 29, 2017 at 19:30.
aeronautics is offline   Reply With Quote

Old   August 29, 2017, 23:10
Default
  #3
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,062
Rep Power: 60
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Try something non-inviscid. You can do slip walls if you want.
LuckyTran is offline   Reply With Quote

Old   August 30, 2017, 06:08
Default
  #4
New Member
 
Hüseyin Emre
Join Date: Mar 2017
Location: Istanbul
Posts: 8
Rep Power: 7
aeronautics is on a distinguished road
Hi LuckyTran ! Thanks for your reply, firstly.

I have tried to use k-e, Standart Wall Fn and no slip by setting specified shears as zero Pascal. It diverged rapidly. Then Ive reduced the URFs by half, it did not affect. I also got "time step reduced ..." warning. Please check how residuals acted.

http://imgur.com/p4ZG5gQ
aeronautics is offline   Reply With Quote

Old   August 31, 2017, 17:57
Default
  #5
New Member
 
Hüseyin Emre
Join Date: Mar 2017
Location: Istanbul
Posts: 8
Rep Power: 7
aeronautics is on a distinguished road
I read that if the model has considerable subsonic region, it may be wise to use pressure-based solver instead of density-based. My flow problem has subsonic region due to exit domain so I used pressure-based solver with reduced URFs. In this time, x,y velocities and energy residuals converged to 1e-5 level yet continuity diverged on the contrary.

Any idea will be welcomed
aeronautics is offline   Reply With Quote

Old   September 1, 2017, 01:22
Default
  #6
Senior Member
 
Alexander
Join Date: Apr 2013
Posts: 2,194
Rep Power: 31
AlexanderZ will become famous soon enoughAlexanderZ will become famous soon enough
Quote:
Originally Posted by aeronautics View Post
I read that if the model has considerable subsonic region, it may be wise to use pressure-based solver instead of density-based. My flow problem has subsonic region due to exit domain so I used pressure-based solver with reduced URFs. In this time, x,y velocities and energy residuals converged to 1e-5 level yet continuity diverged on the contrary.

Any idea will be welcomed
For such kind of simulations the mesh quality plays a big role.
You may try to refine your mesh in the region of flow shocks.

There is a tricky approaches:
1. You may patch the region of subsonic part (before nozzle) with expected pressure.
2. You may use transient simulation with small time-step instead of steady-state. The value of time-step depends on flow speed. For example you may try 1e-05sec as a first case.
Transient solution may be considered as steady-state, when imaginary particle will cross your domain two times because of flow.

Best regards,
Zorin Alexander
AlexanderZ is offline   Reply With Quote

Old   August 30, 2018, 03:57
Smile
  #7
New Member
 
Ravi
Join Date: Aug 2018
Posts: 1
Rep Power: 0
RAVI RANJAN is on a distinguished road
Hi Emre,
It will never converge as you are assigning nozzle exit pressure as ambient pressure but in your case, it will be definitely much higher. First you calculation nozzle exit pressure based on chamber pressure (inlet), expansion ratio and lambda. You may find the standard equation for the nozzle in any relevant book. You use that pressure as pressure outlet and you won't face divergence issue.

If you really would like to simulation a condition where nozzle exit is open in ambient, there you need to add an extra domain after nozzle exit and there you may define that as pressure outlet equal to 101325 pa.
I hope it will help.

Best wishes,
Ravi
RAVI RANJAN is offline   Reply With Quote

Reply

Tags
compressible flow, nozzle

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
PEMFC model with FLUENT brahimchoice FLUENT 22 April 19, 2020 16:44
[ANSYS Meshing] Help with element size sandri_92 ANSYS Meshing & Geometry 14 November 14, 2018 08:54
Convergent Divergent Nozzle Hrishikesh Main CFD Forum 12 June 25, 2016 03:06
fluent divergence for no reason sufjanst FLUENT 2 March 23, 2016 17:08
Convergent Divergent Nozzle with Separation ookalkan CFX 0 January 31, 2011 18:12


All times are GMT -4. The time now is 17:44.