CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   Nozzle Flow - Divergence Problem (https://www.cfd-online.com/Forums/fluent/42152-nozzle-flow-divergence-problem.html)

 Ijaz August 27, 2006 14:26

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 k-e 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 far-field 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

 MKP August 28, 2006 03:48

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

 Raj Kiran Grandhi August 28, 2006 19:58

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 pressure-outlet boundary conditions at all boundaries except the nozzle-inlet unless you are modelling a nozzle flow in an external free-stream

5. Try initializing the solution from the nozzle-inlet, or with values corresponding to the nozzle-throat.

6. You might want to switch over to first-order discretization initially and go to second order after the solution has stabilized.

Hope this helps, Regards, Rajkiran

 d.vamsidhar August 30, 2006 23:22

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

 Ijaz September 1, 2006 05:11

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 9.0245e-01 5.8171e-01 2.8301e+01 1.1260e+00 5.1750e-02 1.1421e-01 24:33:23 4863

reversed flow in 23 faces on pressure-outlet 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 4.9050e-02 1.5255e+00 24:30:11 4862

reversed flow in 69 faces on pressure-outlet 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 1.8637e-02 2.1174e-02 24:11:22 4861

reversed flow in 92 faces on pressure-outlet 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

 MKP September 5, 2006 04:45

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

 javadi September 18, 2006 03:37

Re: Nozzle Flow - Divergence Problem

hello please send me this file very very tank you

 sach October 9, 2006 03:50

Re: Nozzle Flow - Divergence Problem

a5re you solving fuel injection nozzle flow problem? I have already solved thease types of problems

 zeybi1604 March 13, 2012 13:38

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.

 tppraj January 11, 2014 05:36

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 16:49.