CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   water Nozzle modeling (https://www.cfd-online.com/Forums/cfx/93349-water-nozzle-modeling.html)

 agastyamit October 12, 2011 09:06

water Nozzle modeling

i have been trying to model a #flatjet water nozzle#, as it is not an inbuilt option in cfx. There are other particle injection options like full cone etc.

i had to make a fine mesh in the region of the injection..

i am having troubles with the small size particles (200 micron and less), the solution doesnot converge and gives absurd result.. the same with bigger particles (400 micron and so) works good..

does anyone has some idea in this respect???

thanks a lot

 ghorrocks October 12, 2011 19:15

Please show an image of the "absurd" result and convergence details from your out file.

 agastyamit October 13, 2011 07:41

2 Attachment(s)
here is the imge of the result for 200 micron water droplets, height is 1m
direction of water spray is negative y.
also notice the velocity of drops

 ghorrocks October 13, 2011 08:06

What do the 400 micron drops look like? What is it meant to look like?

 agastyamit October 13, 2011 08:13

1 Attachment(s)
this is how 400 micron result looks like ...

there is a spread of drops over about 30 degree angle as should be according to the input
and also spray is flat towards negative y, unlike the one for 200 micron

 agastyamit October 13, 2011 08:13

also note the velocity of the drops

 Graham81 October 13, 2011 08:39

Did you check mesh sensitivity? When the liquid phase (ie the droplet) occupies a significant amount of the cell, the assumptions for the conservation equations of the eulerian phase become invalid. I can imagine that with a fine mesh and increased droplet size, that is what happened.

- Is your minimum cell size in the order of the 400 micron?
- Does coarsening the mesh in that area fix the issue?

Im curious to find out if that was the problem.

 agastyamit October 13, 2011 08:52

the size of the smallest cell is in the range of 100 microns actually!!!!

but the problem is that i am getting acceptable result and convergence for 400 micron particles and not for 200 micron and smaller.

i did not think about this, but there is a reason why i had to make finer mesh in the region of particle injection. I am using a CEL function to define particle injection direction, and need the fine mesh because the function dependce on space variable x. As the droplet injection direct in one cell remains the same the function value can only be changed over variable x if i have fine cells in this direction.

i have noticed that the need of fine mesh doesnot arise in case of in built particle injection methods like full cone or point cone etc...

i dont understand what should i do then????

 agastyamit October 13, 2011 10:37

1 Attachment(s)
i am attaching the ccl file as zip. for the problem i am trying.

the flow rate and nozzle radius are standard values considered for the study of flow from this kind of a nozzle under transverse air flow.

please suggest any mistakes or better way to present the problem.

Thanks a lot

 Graham81 October 13, 2011 10:42

Do I understand correctly you do not model primary breakup but are injection 1 size droplets across a range of angles through your CEL function?

What are you using in terms of secondary breakup and drag deformation models? The 200 micron particles will have significantly different Weber numbers.

If you are merely tracking liquid particles with a constant diameter, it might be worthwile to check whether you are injecting the correct massflow. You will have to inject 8 times the number of droplets in the 200 micron case to get the same massflow, right?

 agastyamit October 13, 2011 11:01

yes i am injecting particles of one dia at different angles governed by CEL function.

for this model i did not use any secondary particle breakup either but i think i need to use some secondary breakup.. you are right weber number for these particles is quit high as the injection velocity is high.

for drag i have used schiller naumann.
i have given a surface tension of 0.72 N/m

while changing the particle size from 400 to 200 micron or any other.. i keep the same massflow.. i think it will be reflected with the number of total particles.. (assuming it is reasonable)!!!

 ghorrocks October 13, 2011 17:47

My first guess would be a numerical round off problem. Try running it with double precision numerics. If you have micron sized cells expanding out to mm sized cells (a size ration of 1:1000) that is always going to be a challenge numerically. You should try to avoid this if possible.

It is not clear to me why you need such a fine mesh anyway.

 agastyamit October 14, 2011 08:49

i need to inject particles from a flatjet nozzle (this kind of a nozzle sprays drops in a plane unlike from a conical nozzle). This is no an inbuilt particle injection option in CFX.

What i am doing is injecting the particles at the top boundary with line weighting of length 1mm (radius of nozzle) and i need to specify a certain deviation. and over this 1mm i am defining a CEL function for injection angle, to make it fan shaped in this plan. I have noticed that the implementation of this space dependent fucntion is possible only if i have enough cells withing this 1mm line. (as a result i need small sized particles)

Could you please suggest me if there is another way i can model the above described nozzle?

thanks a lot

 Graham81 October 14, 2011 10:01

This depends on the purpose of your study. Are you trying to model injection and breakup through a specific nozzle or are you assuming a nozzle effect and just interested tracking droplets through the domain?

If you are after modeling the breakup:

Since you are only injecting seperate droplets, I assume you are in the atomization regime for primary breakup. From the CFX manual:

For the Blob, Enhanced Blob, and the LISA model, the initial injection spray angle needs to be specified explicitly, while for the Turbulence Induced Atomization model, the spray angle is computed within the model.

Blob and Enhanced Blob will be for lower Weber numbers I suspect, LISA assumes a pressure swirl injector (a sheet of liquid at the injector walls), and the Turbulence Induced Model I dont know.

If you are after trajectories, your approach seems the way to go. Perhaps its possible to append the conical injector model already there to include only a planar part of it.

PS: droplet diameter and angles are commonly assumed to fit statistical distributions (eg Rosin Rammler)

 agastyamit October 31, 2011 12:34

hi
thanks for the advice, i need to track the particles (not so much worried about secondary breakup, i am going to include primary breakup)

i have another question related to CFX post in ANSYS

i have generated a Chart with distribution of say particle diameter or particle avg volume fraction vs Variable 'x', what i need is to get is the values in table form.

i have treid to generate table, but i realized that i need to have a lot of points to use a probe function. can anyone suggest me otherwise.

Thanks

 Graham81 November 3, 2011 05:24

If you are injecting droplets with your CEL function, then that is you primary breakup model. Any onward dispersion and particle tracking will start from how you distribute mass, momentum and angles across your sample of droplets at the injector.

Im not sure if what you want is possible in CFX-post, but it can be done in Ensight.

 ghorrocks November 3, 2011 06:23

This should be easy in CFD-Post.

 agastyamit November 3, 2011 10:16

thanks it works in cfd post.. i got it

 All times are GMT -4. The time now is 00:17.