Nozzle Flow  Divergence Problem
Hi all, I am solving a convergent divergent 2D nozzle flow problem, in which the computational domain has been extended well beyond the nozzle boundaries (in both x and y directions) to see any shock waves forming at the nozzle exit and also to see the temperature distribution after the nozzle exit. My mesh looks fine and mesh checking via Gambit does not indicate any bad cells. I am using ke RNG non equilibrium wall functions with inlet and outlets defined as pressure inlet and outlets respectively. However I have taken outlet at the end of mesh (in x direction) instead of nozzle outlet and in y direction, at the end of the mesh, I have used farfield pressure conditions. My solution starts well but after almost 80 iterations, divergence appears and I get temeperature and pressure limitation indication in few cells and then residulas jump to the peak and thats it, solution stops with the error.
Previously, I have been able to solve the same problem in which I used the same mesh but used it only for the case of nozzle itself and didn't exted its boundaries. I wonder if there is anyone who could help me. Thanks, Ijaz 
Re: Nozzle Flow  Divergence Problem
Well Ijaz, it used to happen when u extend ur domain from nozzle outlet.
At first where do u expect the shock....! Accordingly u widen & lengthen ur domain from nozzle outlet. Then, check whether mesh is structured one. while solving, Use low under relaxation till the convergence...! so ur problem will take bit longer time to converge..! all the best, MKP 
Re: Nozzle Flow  Divergence Problem
1. What solver are you using? If you are using the segregated solver, try switching to the coupled implicit solver.
2. Reduce the courant number to 0.1 or so at the beginning of the solution. 3. Try to use a structured mesh if possible 4. Try giving a pressureoutlet boundary conditions at all boundaries except the nozzleinlet unless you are modelling a nozzle flow in an external freestream 5. Try initializing the solution from the nozzleinlet, or with values corresponding to the nozzlethroat. 6. You might want to switch over to firstorder discretization initially and go to second order after the solution has stabilized. Hope this helps, Regards, Rajkiran 
Re: Nozzle Flow  Divergence Problem
dear ijaz, the residuals will converge either you use pressure far feild boundary condition or outlet vent for the outer domain and the pressure outlet for the exit of the domain perpendicular to flow direction. also start the under relaxation factors from 0.4 for most and for pressure start with 0.2 and for momentum start .use segregated solver and SA MODEL. regards, d.vamsidhar

Re: Nozzle Flow  Divergence Problem
Thank you MKP, Raj Kiran and d.vamsidhar for your suggestions, I have tried most of what was suggested by MKP and Raj with no avail.
I am using coupled implicit solver, because of the contour of the nozzle, its not possible for me to have a structured mesh (or perhaps I am not very good at it). I reduced the courant number to 0.1 and used 1st order discrteisation (as suggested) for about first 150 iterations and then increased the courant number to 5 with all discretisations to 2nd order and this is what I get after few more iterations, just before the solution stops (Mind that I had also increased the limits of absolute pressure and temperature to an on order to avoid divergence): time step reduced in 12 cells temperature limited to 5.000000e+004 in 1 cells on zone 2 288 9.0245e01 5.8171e01 2.8301e+01 1.1260e+00 5.1750e02 1.1421e01 24:33:23 4863 reversed flow in 23 faces on pressureoutlet 7. time step reduced in 10 cells absolute pressure limited to 1.000000e+000 in 1 cells on zone 2 temperature limited to 5.000000e+004 in 1 cells on zone 2 289 1.1743e+00 1.9025e+00 2.8995e+01 3.0353e+00 4.9050e02 1.5255e+00 24:30:11 4862 reversed flow in 69 faces on pressureoutlet 7. time step reduced in 68 cells absolute pressure limited to 1.000000e+000 in 1 cells on zone 2 temperature limited to 5.000000e+004 in 3 cells on zone 2 290 1.3929e+00 1.5426e+02 1.5782e+03 2.8637e+02 1.8637e02 2.1174e02 24:11:22 4861 reversed flow in 92 faces on pressureoutlet 7. divergence detected  temporarily reducing Courant number to 0.5 and trying again... temperature limited to 5.000000e+004 in 19 cells on zone 2 Error: Floating point error: invalid number So far I have not played with the under relaxation factors, will try it now as suggested and let you know what do I get. Thank you all once again, Ijaz 
Re: Nozzle Flow  Divergence Problem
Hi,
150 iterations is very small number..The solver would have not digested ur initial and boundary conditions...! It is better to go 1000 iterations with courant no.0.1 and under relaxation of 0.1.. Then, SLOWLY INCREASE the courant number from 0.1 to 1 and then 1 to 5... Set the limit correctly.. all the best. MKP 
Re: Nozzle Flow  Divergence Problem
hello please send me this file very very tank you

Re: Nozzle Flow  Divergence Problem
a5re you solving fuel injection nozzle flow problem? I have already solved thease types of problems

multiphase flow( 2phase) unsteady mixture model
has anyone done a 2 phase simulation inside a packed and has it working properly without any error messages obtained like "divergence in AMG solver:x momentum".thank u in advance.

Nozzle floe
Friends,
I am trying to converge the nozzle flow, for that extended domain is choose and density based implicit solver is used. I am using structured grid but after several iterations the temperature limit ( error ) message is shown. Will you please help to converge this problem. 
All times are GMT 4. The time now is 08:19. 