CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   Euler Lagrange Convergence Tips (

snpradeep May 6, 2013 06:02

Euler Lagrange Convergence Tips
I am doing spray simulation in a pipe. Where nozzle is placed coaxial to the pipe with the help of an elbow. The pipe is approx. 3m long and
The bc of sim are as follows..
At inlet velocity profile is used with a static temp of 350 C (Approx 4.65 bars) to account for secondary flow inside the testrig
At outlet Avg static pr. of 4.63 bar is specified.

For particles Injection parameters are spec acc to lisa computations.
Breakup length approx. 1mm
Radius at breakup 0.7mm
Vel Magnitude 121 m/s
Injection type: Discrete Diameter distribution. (Approx Rosin Rammler Dia 51 micron and spread approx 3.75)
No. of Rep Particles: 100000
Unfortunately I am not able to get converged results..After approx 100 iterations solver diverges...
My particle solver setup is as follows..
First Iteration for Particle Calculation = 300
Iteration Frequency = 10
Maximum Particle Integration Time Step = 1.0E10 [s]
Number of Integration Steps per Element = 100
Option = Forward Euler
Option = Smooth
Maximum Number of Integration Steps = 100000
Maximum Tracking Distance = 2 [m]
Maximum Tracking Time = 10 [s]
Energy Under Relaxation Factor = 0.5
Energy Under Relaxation Factor for First Particle Integration = 0.5
Mass Under Relaxation Factor = 0.5
Mass Under Relaxation Factor for First Particle Integration = 0.5
Velocity Under Relaxation Factor = 0.5
Velocity Under Relaxation Factor for First Particle Integration = 0.5
Option = Smooth
Rhie Chow Option = High Resolution

I have tried many trials by changing relaxation factors up to 0.1 for particles and Iteration frequency up to 25 but still no success.
Also one thing i noticed was.. When I deactivate turbulent dispersion of partilces I get a good convergence. When I activate turbulent dispersion my simulation keeps on diverging. Any tips would be of great help.

ghorrocks May 6, 2013 06:21

Are you sure you have your reference pressure and boundary pressures set correctly? This simulation sounds like it needs a reference pressure of 4.63 bar, an inlet of 0.02 bar and outlet of 0 bar.

Aer you sure you need to model this as a particle tracking model? If you want to model breakup then I guess you have to. But if the Eualrian model is applicable it can be much easier to use and run.

Forget your previous SIMPLE solver experience and stop fiddling with under relaxation factors. It is extremely rare that you need to adjust these in CFX. If you are not getting convergence it is not due to tunder relaxation factors but a more fundamental problem with your simulation. Likewise for Rhie Chow - leave this at default.

My recommendation is to make sure this converges without the spray on first. In fact you should do a sensitivity analysis on this basic flow first to ensure that you are modellign the single phase flow OK before proceeding. One that is done turn the spray on, initially with just a few particles and no spray break up or turbulent dispersion. Then add the physics one bit at a time - first the spray break up, then the turbulent dispersion, then anything else. Make sure each bit is working correctly before proceeding.

And there is comments in the CFX documentation about convergence with turbulent dispersion - I recommend you read it. It will tell you why you are not converging with it.

snpradeep May 6, 2013 07:15

Dear ghorrocks,

Continuousphase is working fine..My Inlet bc is Velocity magnitude (Which uses a velocity profile). This velocity profile was obtained by a transient sim of the entire testrig. At Exit I have pressure of 4.63bar.. And ref pressure of 0 bars. Which gives me 4.65 bars of pressure at inlet Which fairly match with experiments. The only problem I face is with particles..When I inject many particles I face this problem of convergence..(above 10000 particles). Thank you verymuch for the reply. I will take your advice and rebuild the simulation..


All times are GMT -4. The time now is 08:51.