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

shocks in convergent divergent nozzle, convergence issue

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 30, 2019, 06:36
Default shocks in convergent divergent nozzle, convergence issue
  #1
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
hi!
i was doing a simulation of convergent divergent nozzle , fluid taken as air , pressure at inlet and pressure at outlet is known. I want an efficient combination of convergent and divergent angle to have min drag on the incoming fluid. taken viscous fluid, energy equation is ON.

OK, now coming to problem.
first I did the steady state analysis and I found that the solution didn't converge due formation of eddies in the divergent section. So I went with a transient simulation and monitored Cd plot. It was seen that series shocks were produced in the divergent section. As Cd plot converged I tried to converge the solution at a particular time step, as I thought that the oscillation of residual between 1e-04 and 1e-05 is due the eddies in the flow.

so I used time step size = 0.1s
time steps = 1
and increased the no. of iteration/time step in order to converge the solution below 1e-06.

but I found that the residual fall a little but didn't converged below 1e-06, residual started oscillating around 1e-05.

but when I reduced the time step to 1e-05 the solution converged below residuals 1e-06.
I don't understand why the model is showing such a behaviour. is it due to shocks or the eddies?

Any help is appreciated
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   December 30, 2019, 10:47
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
You wrote a lot of things that, however, are of no help.
What about:
1) 2d/3d geometry
2) Formulation of the governing equations
3) Numerical discretization/software
4) BCs. setting


and, would be of some help if you post some result.
FMDenaro is offline   Reply With Quote

Old   December 30, 2019, 12:02
Default
  #3
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
You wrote a lot of things that, however, are of no help.
What about:
1) 2d/3d geometry
2) Formulation of the governing equations
3) Numerical discretization/software
4) BCs. setting


and, would be of some help if you post some result.
1. 2D geometry with axisymmetric assumption
2. Navier stokes eqs with transition SST model, density based solver.
3. Ansys fluent
4. Bcs. pressure inlet = 101325 pa , T = 298 K
pressure outlet = 33800 pa
wall :- no slip, heat flux = 0
axis
Attached Images
File Type: jpg geometry.jpg (95.3 KB, 20 views)
File Type: jpg mesh.jpg (165.6 KB, 20 views)
File Type: jpg residuals plot.jpg (112.3 KB, 16 views)
File Type: jpg cd plot.jpg (99.5 KB, 15 views)
File Type: jpg streamlines.jpg (90.4 KB, 25 views)
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   December 30, 2019, 12:26
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Well, due to the axisymmetric assumption and the RANS modelling, the existence of a time-dependent fluctuation in the eddies has no physical meaning.
What I see is that you have a subsonic inflow (one condition must be set free to adapt from the interior) but the outflow is a mix of supersonic/subsonic flow regions. That should be one of the reasons of the convergence problem.
As you did not write nothing about the numerical integration in time and space, I can suppose also problems in the numerical stability constraints.
Furthermore, the turbulence model could add problems.
However, to check the viscous drag you should have a wall-resolved grid.



I strongly suggest to run first a standard test-case and check if you are able to produce a good solution.
FMDenaro is offline   Reply With Quote

Old   December 30, 2019, 15:18
Default
  #5
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
Well, due to the axisymmetric assumption and the RANS modelling, the existence of a time-dependent fluctuation in the eddies has no physical meaning.
What I see is that you have a subsonic inflow (one condition must be set free to adapt from the interior) but the outflow is a mix of supersonic/subsonic flow regions. That should be one of the reasons of the convergence problem.
As you did not write nothing about the numerical integration in time and space, I can suppose also problems in the numerical stability constraints.
Furthermore, the turbulence model could add problems.
However, to check the viscous drag you should have a wall-resolved grid.



I strongly suggest to run first a standard test-case and check if you are able to produce a good solution.
Thank you for your reply.
I am not able to follow your second point can you please elaborate.
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   December 30, 2019, 15:25
Default
  #6
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by yogeshghadge314@gmail.com View Post
Thank you for your reply.
I am not able to follow your second point can you please elaborate.
What exactly?
FMDenaro is offline   Reply With Quote

Old   December 30, 2019, 23:35
Default
  #7
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
What exactly?
Having a subsonic flow at inlet and mixed subsonic/supersonic flow at outlet, how does it leads to convergence problem?
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   December 31, 2019, 04:34
Default
  #8
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by yogeshghadge314@gmail.com View Post
Having a subsonic flow at inlet and mixed subsonic/supersonic flow at outlet, how does it leads to convergence problem?

According to the characteristic directions, supersonic outflow has different BC setting from a subsonic outflow. If the eddies at the outflow cause the fluctuation of the Mach number at the outlet, the solver can have problem in convergence.
On the other hand you are integrating in time and further problems can be in the numerical stability, check the correct CFL.
However, without details about the numerical integration is difficult to see your problem.
Again, solve first a well assessed test-case from the literature.
FMDenaro is offline   Reply With Quote

Old   December 31, 2019, 08:32
Default
  #9
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
According to the characteristic directions, supersonic outflow has different BC setting from a subsonic outflow. If the eddies at the outflow cause the fluctuation of the Mach number at the outlet, the solver can have problem in convergence.
On the other hand you are integrating in time and further problems can be in the numerical stability, check the correct CFL.
However, without details about the numerical integration is difficult to see your problem.
Again, solve first a well assessed test-case from the literature.
I read about this problem a bit. It was said that the time dependent oscillations are due to the shock-boundary layer interaction which is an unsteady phenomenon. The position of the shocks tends to move to and fro by a slight amount which brings an unsteady behaviour in the model.
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   December 31, 2019, 09:32
Default
  #10
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 425
Rep Power: 18
JBeilke is on a distinguished road
A time step size of 0.1s is simply too big. Adjust this value the get a courant number somwhere between 0.5 and 5 (depends on the solver).



@FMD
He is using the normal Fluent settings and this is a well defined testcase. No need to be overacademic.
JBeilke is offline   Reply With Quote

Old   December 31, 2019, 09:37
Default
  #11
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by JBeilke View Post
A time step size of 0.1s is simply too big. Adjust this value the get a courant number somwhere between 0.5 and 5 (depends on the solver).



@FMD
He is using the normal Fluent settings and this is a well defined testcase. No need to be overacademic.





Using a viscous and turbulent model in this test case is quite redundant to be really a test-case. First of all he should be able to get a steady solution in standard conditions for checking the BC.s setting.

Then, using the axisymmetric condition is valid for a statistically steady flow. In case of a physical description of the oscillations, the gemoetry must be 3D.
Thus, I see too many mixed issues in this problem.
FMDenaro is offline   Reply With Quote

Old   December 31, 2019, 10:40
Default
  #12
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
@Jbeilke @FMD
Thank you both for your reply. I will consider your suggestions and perform the simulation again.
@FMD
Can you please explain why the flow should be statically steady for axisymmetric assumption.
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   December 31, 2019, 11:11
Default
  #13
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by yogeshghadge314@gmail.com View Post
@Jbeilke @FMD
Thank you both for your reply. I will consider your suggestions and perform the simulation again.
@FMD
Can you please explain why the flow should be statically steady for axisymmetric assumption.

Fluctuations in a real turbulent field are not axisymmetric even if the geometry is axisymmetric. For this reason what you see is numerical, not a real physical aspect of the flow.
FMDenaro is offline   Reply With Quote

Old   January 1, 2020, 04:01
Thumbs up
  #14
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
Fluctuations in a real turbulent field are not axisymmetric even if the geometry is axisymmetric. For this reason what you see is numerical, not a real physical aspect of the flow.
Thanks. Got it
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   January 1, 2020, 07:06
Default
  #15
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
You can find in literature papers about the turbulent flow structures in a converging-diverging nozzle, using DNS/LES/URANS.
But I suggest to check if you are able to replicate this test case
https://www.researchgate.net/publica...d_Dynamics_CFD
FMDenaro is offline   Reply With Quote

Old   January 2, 2020, 05:59
Default
  #16
New Member
 
Howwikis
Join Date: Dec 2019
Posts: 1
Rep Power: 0
Howwikis is on a distinguished road
United States Banking
Howwikis is offline   Reply With Quote

Old   January 2, 2020, 09:59
Default
  #17
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
Quote:
Originally Posted by FMDenaro View Post
You can find in literature papers about the turbulent flow structures in a converging-diverging nozzle, using DNS/LES/URANS.
But I suggest to check if you are able to replicate this test case
https://www.researchgate.net/publica...d_Dynamics_CFD
Thanks, I will take a look.
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   January 2, 2020, 10:40
Default
  #18
New Member
 
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5
yogeshghadge314@gmail.com is on a distinguished road
@FMD
I tried to set the time step by CFL based time setting. It is showing that the time step required for courant no. to be 1 is 6e-10 s. which is too small and taking a very large computational time for the solution to converge. But on the positive side, the solution is showing sign of convergence.
yogeshghadge314@gmail.com is offline   Reply With Quote

Old   January 2, 2020, 11:55
Default
  #19
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67
FMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura aboutFMDenaro has a spectacular aura about
Quote:
Originally Posted by yogeshghadge314@gmail.com View Post
@FMD
I tried to set the time step by CFL based time setting. It is showing that the time step required for courant no. to be 1 is 6e-10 s. which is too small and taking a very large computational time for the solution to converge. But on the positive side, the solution is showing sign of convergence.

Not strange at all, the CFL take into account acustic waves for the stability of explicit method.

Generally, an implicit method is used in order to adopt a greater time-step. However, try to reach a convergent solution with this small time-step before to proceed further with change in the setting.
FMDenaro is offline   Reply With Quote

Old   January 2, 2020, 17:54
Default
  #20
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 425
Rep Power: 18
JBeilke is on a distinguished road
The time step size for Co=1 should not be so small. There are some error messages on the mesh picture. Please check the mesh quality at first.
JBeilke is offline   Reply With Quote

Reply

Tags
convergent-divergent, shocks

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
Problem: Convergent- Divergent Nozzle Venting to Atmosphere JohnPeclet FLUENT 2 January 13, 2015 19:57
Convergent nozzle and preesure of steam pranabjyoti CFX 7 March 10, 2011 20:23
Convergence issue in SST for Porous model Raj CFX 0 May 2, 2008 03:43
CFX-Solver, issue with convergence behavior Andy CFX 7 September 5, 2006 04:24
compressible flow in a counterflow nozzle d.vamsidhar FLUENT 0 November 24, 2005 02:45


All times are GMT -4. The time now is 05:58.