
[Sponsors] 
shocks in convergent divergent nozzle, convergence issue 

LinkBack  Thread Tools  Search this Thread  Display Modes 
December 30, 2019, 06:36 
shocks in convergent divergent nozzle, convergence issue

#1 
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 
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 1e04 and 1e05 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 1e06. but I found that the residual fall a little but didn't converged below 1e06, residual started oscillating around 1e05. but when I reduced the time step to 1e05 the solution converged below residuals 1e06. I don't understand why the model is showing such a behaviour. is it due to shocks or the eddies? Any help is appreciated 

December 30, 2019, 10:47 

#2 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 
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. 

December 30, 2019, 12:02 

#3  
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 
Quote:
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 

December 30, 2019, 12:26 

#4 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 
Well, due to the axisymmetric assumption and the RANS modelling, the existence of a timedependent 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 wallresolved grid. I strongly suggest to run first a standard testcase and check if you are able to produce a good solution. 

December 30, 2019, 15:18 

#5  
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 
Quote:
I am not able to follow your second point can you please elaborate. 

December 30, 2019, 15:25 

#6 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 

December 30, 2019, 23:35 

#7 
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 

December 31, 2019, 04:34 

#8  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 
Quote:
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 testcase from the literature. 

December 31, 2019, 08:32 

#9  
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 
Quote:


December 31, 2019, 09:32 

#10 
Senior Member
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 425
Rep Power: 18 
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. 

December 31, 2019, 09:37 

#11  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 
Quote:
Using a viscous and turbulent model in this test case is quite redundant to be really a testcase. 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. 

December 31, 2019, 10:40 

#12 
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 
@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. 

December 31, 2019, 11:11 

#13  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 
Quote:
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. 

January 1, 2020, 04:01 

#14 
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 

January 1, 2020, 07:06 

#15 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 
You can find in literature papers about the turbulent flow structures in a convergingdiverging 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 

January 2, 2020, 05:59 

#16 
New Member
Howwikis
Join Date: Dec 2019
Posts: 1
Rep Power: 0 

January 2, 2020, 09:59 

#17  
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 
Quote:


January 2, 2020, 10:40 

#18 
New Member
CFD online
Join Date: Dec 2019
Posts: 9
Rep Power: 5 
@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 6e10 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. 

January 2, 2020, 11:55 

#19  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,259
Rep Power: 67 
Quote:
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 timestep. However, try to reach a convergent solution with this small timestep before to proceed further with change in the setting. 

January 2, 2020, 17:54 

#20 
Senior Member
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 425
Rep Power: 18 
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.


Tags 
convergentdivergent, shocks 
Thread Tools  Search this Thread 
Display Modes  


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 
CFXSolver, 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 