spray injection problems
 

I was doing the spray injection simulation.
Water droplets was injected in the static air occupied cylinder by pressure-swirl atomizer with on inlet and pressure outlet.
LISA model and ETAB model was employed.

The parameters for the atomizer to abotain the initial condition of the droplets was;
deltap=0.9MPa cone angle=28.3 radius=1.16mm massflow=0.3251kg/s Density probe normal distance=1mm(I just guess this parameter)


As my understanding,because the continuous phase was static, it should be laminar flow,so no turbulence model should be employed.
But the error message bring up when i run the simulation,that is


" ERROR #002100004 has occurred in subroutine Out_Scales_Flu. |
| Message: |
| The Reynolds number is outside of the range expected based on the |
| Option selected for the TURBULENCE MODEL. Check this setting, |
| the values of the properties, mesh scale, consistency of units |
| and solution values in the input file. Execution will proceed. |
+---------------------------------------------------------------"

Anyone willing to help ,thank you.
I have difficulty in doing this simulation, if someone who have done this kind of work, i am grateful to your advice.

It is not an error, just a warning. If you are confident the flow is laminar then you can ignore it and proceed.

Glenn,thank you.
I have several questions about the my spray injection simulation.

As i know, the fluid phase is governed by the NS equations, and the particle phase by particle kinematics. The particle phase is coupled to the fluid phase using source terms.

And in my simulation,the fluid phase was static initially,so it seems that there is no need to small mesh,the fluid phase feature is easily captured by coarse mesh.
Right?

2)I did this simulation for several days, but it is difficult to converge.
As my previous post depicts ,the physical problem is that water droplets are injected in the static air occupied cylinder by pressure-swirl atomizer with no inlet and pressure outlet.


I simplify the simulation in order to get an easy start and an initial condition for the full simulation.So:

Buoyancy =off; Particle break up=off; particle collision=off


There are several problems:
1.I set the outlet pressure condition, but during the run, there is a message saying i should change it to opening condition.But as my understanding, there is only droplets exit the domain.

2.It is difficult to converge,i have tried to solve it ,but it didn't work.
I think whether is the static fluid condition cause the difficulty to converge?
What should i do,thank you.
Here are the CCL file ,and in the previous post there are out file.
Thank you for your patience, you help makes a difference.

Your simulation is clearly not happy, it is saying you have back flow in around 90% of your outlet. Either move the boundary somewhere the flow is in a known direction or use a opening.

Also this FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

Thanks ,Glenn.
But it should not exist back flow as there are only droplets exit domain.
What about this quetion;
"And in my simulation,the fluid phase was static initially,so it seems that there is no need to small mesh,the fluid phase feature is easily captured by coarse mesh.
Right?"
Besides i have read the link.
I am trying to work it out.

If the boundary is into ambient air then there will be regions of inflow and regions of outflow. The air flows will be weak, but present never the less. This type of boundary is better done as an opening, not an outlet.

You should determine the mesh size your model requires with a sensitivity analysis. Start with an educated guess, sure, but then refine it and coarsen it until you find what it really requires.

Glenn，thanks.
But the problem is that it can'y obtain fully converged, so how can i determine the proper mesh in advance?
And in the out file, i saw the Reynolds number is 8.7477E+04.
How can that possible?under this number,laminar flow is not suitable.
And when i turn turbulence to k-e model,it obtain fully convergence ,Is it physically real?

You have to have a simulation which converges reliably before considering mesh size.

Don't worry about the Re number reported in the out file. It is not important for your model. Look at the non-dimensional numbers relevant to your flow to determine what flow regime it is in, and set the models (eg turbulent versus laminar) accordingly.

As i know we sue the Reynolds number to judge what flow regime it is.Isn't it?

Re number is probably the most important non dimensional number in fluid mechanics. It is critical. But it is defined based on a length, velocity and fluid properties scale - and where does that come from? A person can easily pick the important length scales (eg the diameter of a pipe, distance along a surface) and velocity scale (eg centre line velocity, free stream velocity) but a computer does not know this.

So CFX works out a default Re number using the cube root of the total domain volume for a length scale, some form of global average for the velocity scale and fluid property scales. So the calculated Re number is not based on useful scales, and therefore is not comparable with the Re numbers you know from pipe flow or boundary layer growth.

So if you want a Re number from your flow which means something you have to do the calculation yourself with an appropriate length, velocity and fluid property scales.

Glenn,thank you.
I got it.
I assume it was a turbulent flow and will do literate work to determine finally.
Now i was doing the sensitivity analysis of the "numbers of positions",cause i think it is an important parameter.
I start the number from 1000, and i want to set the averaged Sauter mean particle in the volume as the monitor.
I first thought the CEL:
volumeAve(water.Averaged Sauter Mean Particle Diameter)@REGION:SOLID
But it seems it isn't the right expression.
Can you help me ?