CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

water Nozzle modeling

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   October 12, 2011, 09:06
Default water Nozzle modeling
  #1
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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
agastyamit is offline   Reply With Quote

Old   October 12, 2011, 19:15
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Please show an image of the "absurd" result and convergence details from your out file.
ghorrocks is online now   Reply With Quote

Old   October 13, 2011, 07:41
Default
  #3
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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
Attached Images
File Type: jpg 200 micron flatjet.jpg (63.2 KB, 124 views)
File Type: jpg momentum convergence.jpg (92.5 KB, 86 views)
agastyamit is offline   Reply With Quote

Old   October 13, 2011, 08:06
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What do the 400 micron drops look like? What is it meant to look like?
ghorrocks is online now   Reply With Quote

Old   October 13, 2011, 08:13
Default
  #5
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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
Attached Images
File Type: jpg 400 micron flatjet.jpg (81.1 KB, 93 views)
agastyamit is offline   Reply With Quote

Old   October 13, 2011, 08:13
Default
  #6
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
also note the velocity of the drops
agastyamit is offline   Reply With Quote

Old   October 13, 2011, 08:39
Default
  #7
Member
 
Join Date: Dec 2009
Posts: 57
Rep Power: 7
Graham81 is on a distinguished road
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.
Graham81 is offline   Reply With Quote

Old   October 13, 2011, 08:52
Default
  #8
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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 is offline   Reply With Quote

Old   October 13, 2011, 10:37
Default
  #9
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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
Attached Files
File Type: zip flatjet 200 micron.zip (3.9 KB, 39 views)
agastyamit is offline   Reply With Quote

Old   October 13, 2011, 10:42
Default
  #10
Member
 
Join Date: Dec 2009
Posts: 57
Rep Power: 7
Graham81 is on a distinguished road
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?
Graham81 is offline   Reply With Quote

Old   October 13, 2011, 11:01
Default
  #11
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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)!!!
agastyamit is offline   Reply With Quote

Old   October 13, 2011, 17:47
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is online now   Reply With Quote

Old   October 14, 2011, 08:49
Default
  #13
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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
agastyamit is offline   Reply With Quote

Old   October 14, 2011, 10:01
Default
  #14
Member
 
Join Date: Dec 2009
Posts: 57
Rep Power: 7
Graham81 is on a distinguished road
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)
Graham81 is offline   Reply With Quote

Old   October 31, 2011, 12:34
Default
  #15
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
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
agastyamit is offline   Reply With Quote

Old   November 3, 2011, 05:24
Default
  #16
Member
 
Join Date: Dec 2009
Posts: 57
Rep Power: 7
Graham81 is on a distinguished road
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.
Graham81 is offline   Reply With Quote

Old   November 3, 2011, 06:23
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,958
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
This should be easy in CFD-Post.
ghorrocks is online now   Reply With Quote

Old   November 3, 2011, 10:16
Default
  #18
New Member
 
Amit Agasty
Join Date: Oct 2011
Location: CLZ, Deutschland
Posts: 15
Rep Power: 5
agastyamit is on a distinguished road
thanks it works in cfd post.. i got it
agastyamit is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Water Evaporation and condensation modeling Linjie CFX 8 April 23, 2015 18:30
Water subcooled boiling Attesz CFX 7 January 5, 2013 04:32
Water Evaporation and condensation modeling Linjie FLUENT 3 February 6, 2012 14:08
Modeling water jet exiting nozzle pluto STAR-CCM+ 1 November 18, 2009 20:41
uptodate water distribution network fredius,magige,tanzanian,(e.a) Main CFD Forum 0 January 27, 2002 08:10


All times are GMT -4. The time now is 18:13.