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

Injection Spray into Air with Opening Pressure of 30bar

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

Like Tree1Likes
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 27, 2018, 16:36
Default Injection Spray into Air with Opening Pressure of 30bar
  #1
Member
 
Join Date: Mar 2018
Posts: 30
Rep Power: 5
Spray_Ansys is on a distinguished road
Hello guys

I'm new here because I need your advice:

Currently, I'm simulating a water spray, which is coming out of a 0.75mm nozzle diameter. The spray injects in a surrounding of air with 30bars opening pressure. Following some details:

Analysis Type:
Steady State
Fluid Definitions:
Air as Ideal Gas, Water, both stationary, non Buoyant, Continuous Fluid
Turbulence:
SST
Inlet:
Inhomogeneous Velocity Profile (CSV-File), average 300 m/s
Opening:
30bars
Wall:
Free Slip Wall
My problem now is, that I can't find a solution which lead my RMS to convergence. I tried physical timescale with 1E-8, but even there, after 500 iteration, the following problem appears: Overflow

I'm using a student licence, which doesn't allow me to exceed the number of nodes of 500'000.
The "mesh quality" may cause some problems or the inhomogeneous velocity profile. But actually, a simulation with opening pressure of 1bar did end successfully.

So, what do you think may solve my problem? Do you have any suggestions or good advice? If you need more information, please let me know!

Thank you for help and replies!
Spray_Ansys is offline   Reply With Quote

Old   March 27, 2018, 19:02
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,645
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Which multiphase model are you using?

Why are you doing the simulation? What are you intending to get out of the results?
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   March 28, 2018, 06:41
Default
  #3
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,323
Rep Power: 20
Gert-Jan will become famous soon enough
Spray, 30 bar, 300 m/s. This is a very complicated case with difficult physics.

Don't try to go for the top from scratch. Start simple: atmospheric & 10 m/s and then gradually increase complexity and see where it fails.
Gert-Jan is offline   Reply With Quote

Old   April 5, 2018, 05:25
Default
  #4
Member
 
Join Date: Mar 2018
Posts: 30
Rep Power: 5
Spray_Ansys is on a distinguished road
I'm using the Standard Free Surface Model with Turbulence Shear Stress Transport .
I'm intending to simulate the spray breakup and its distraction after the nozzle outlet.

However, I reached a full calculation without any error messages. Unfortunately, it didn't come to nice convergence (see picture).
At the iteration of around 890 some of the residuals seem to rise / diverge after they fall below abort criterion of 1E-5. My question is now, why?
I guess it could be: due to the physical timescale, which need to be smaller[/LIST]or the mesh is too imprecise / not too fine for the job.

But, what do you think? Does anyone have some experience with that?
If you have some questions, please don't hesitate to ask me.

I thank for every answer!
Attached Images
File Type: jpg Simulation_071_1000Iterationen_crop.jpg (137.8 KB, 18 views)
Spray_Ansys is offline   Reply With Quote

Old   April 5, 2018, 05:53
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,323
Rep Power: 20
Gert-Jan will become famous soon enough
- Why do you use free surface model. This is for flat surfaces of e.g. water to study waves.........
- is your plan to predict the water droplet size at the outlet? If so, did you include surface tension?
- Regarding the residuals. Can yo ushare the mass and momentum imbalances?
Gert-Jan is offline   Reply With Quote

Old   April 5, 2018, 06:35
Default
  #6
Member
 
Join Date: Mar 2018
Posts: 30
Rep Power: 5
Spray_Ansys is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
- Why do you use free surface model. This is for flat surfaces of e.g. water to study waves.........
- is your plan to predict the water droplet size at the outlet? If so, did you include surface tension?
- Regarding the residuals. Can yo ushare the mass and momentum imbalances?
- Under Default Domain - Fluid Model - Multiphase - Homogeneous Model I didn't check the box. Shall I check it, although nothing is homogeneous (inlet profile)? In this tab I only checked the Turbulence Model.
- No, not the droplet size, just the spray in general.
- I added it in the attachement

Thank you very much for your help Gert-Jan!
Attached Images
File Type: png Attachement.PNG (8.7 KB, 9 views)
Spray_Ansys is offline   Reply With Quote

Old   April 5, 2018, 06:42
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,645
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Is this is what you had in mind? https://www.youtube.com/watch?v=O0aynlUkRBQ

Modelling high pressure spray breakup using a free surface model means you are modelling some seriously difficult physics in minute detail. This is not something for the CFD beginner - you will require careful model development, a supercomputer and a lot of computer time. I have some experience in modelling similar flows and I can assure you it is extremely challenging.

Can I ask why are you modelling this, and what do you intend to learn by doing the simulation?
Gert-Jan likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 5, 2018, 06:49
Default
  #8
Member
 
Join Date: Mar 2018
Posts: 30
Rep Power: 5
Spray_Ansys is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
Is this is what you had in mind? https://www.youtube.com/watch?v=O0aynlUkRBQ

Modelling high pressure spray breakup using a free surface model means you are modelling some seriously difficult physics in minute detail. This is not something for the CFD beginner - you will require careful model development, a supercomputer and a lot of computer time. I have some experience in modelling similar flows and I can assure you it is extremely challenging.

Can I ask why are you modelling this, and what do you intend to learn by doing the simulation?
Thank you ghorrocks for your answer!
Well, this looks really nice, but isn't what I intend to do. It doesn't need to be a animation nor a transient simulation. In my case, everything is stationary. Is there another way to simulate my case, like with another model?

I'm currently doing my bachelor degree in Mechanical Engineering and specialize in Thermo- and Fluid-Engineering.

Thanks for your answers and help so far!
Spray_Ansys is offline   Reply With Quote

Old   April 5, 2018, 06:53
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,645
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
High pressure spray breakup is an inherently 3D transient flow. You cannot model it steady state as you appear to have done so far with a free surface modelling approach.

Can I ask why are you modelling this, and what do you intend to learn by doing the simulation?

The reason I ask this is because there are many other ways of modelling sprays which are FAR easier. Eularian and Lagrangian droplet models are available which are much more reasonable simulations but they require simplifications and assumptions to be made. That is why you need to know what you are trying to learn from the simulation before you can choose an appropriate model.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 5, 2018, 07:05
Default
  #10
Member
 
Join Date: Mar 2018
Posts: 30
Rep Power: 5
Spray_Ansys is on a distinguished road
I'm currently doing my bachelor degree and investigate in my thesis (diploma of the last semester) liquid sprays. I want to know, how sprays change, when some properties (temperature, pressure, viscosity, ... ) will be modified.

The thing is, that the simulation of a homogeneous inlet profile (everywhere the same normal speed of 300 m/s) works properly and with less iteration. When I activate the inhomogeneous inlet velocity profile, everything get more complex.
So, and I solved the spray (see attachment above) and I ask, why the residuals diverge after ~890 Iteration.

Is the model incorrect? Wrong mesh size? Any suggestions?
Spray_Ansys is offline   Reply With Quote

Old   April 5, 2018, 07:39
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,645
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
I want to know, how sprays change, when some properties (temperature, pressure, viscosity, ... ) will be modified.
So I gather by that you want to change the temperature, pressure, viscosity and see the effect on the spray - and does that mean properties like droplet size and distribution, spray penetration and things like that? Please state the properties you are trying to measure in the spray.

There will be literature papers around which have already done this sort of thing, so you just need to dig up the papers and use their results to get the spray properties. There is no need for you to model anything.

Also: CFX has a spray breakup model suitable for this pressure range for lagrangian particle tracking. This model was built for diesel fuel injectors but with a bit of work it should work for your flows. Have you considered using this model rather than a free surface model? It will be MUCH easier to get useful results from this model compared to your current approach.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 5, 2018, 08:18
Default
  #12
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,323
Rep Power: 20
Gert-Jan will become famous soon enough
I fully agree with Glenn. Nevertheless,
- if you want to stick to your plan, don't start with 300 m/s and 30 bar. You can't do what e.g. Bosch Gmbh in germany is trying (!) with a large R&D team and huge cluster. Start with something easier. A bit more down to earth, please.
- if you want to do something like in the youtube movie, you should start doing VOF kind of stuff for which I would recommend fluent or star-ccm+ (or even star-cd). Not CFX.

Good luck, Gert-Jan
Gert-Jan is offline   Reply With Quote

Old   April 5, 2018, 10:42
Default
  #13
Member
 
Join Date: Mar 2018
Posts: 30
Rep Power: 5
Spray_Ansys is on a distinguished road
Thank you for your help and recommendations.
However, does anyone suggest what it means when the residuals are raising after ~890 Iteration?
Spray_Ansys is offline   Reply With Quote

Old   April 5, 2018, 10:59
Default
  #14
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,323
Rep Power: 20
Gert-Jan will become famous soon enough
Impossible to say since your mass imbalance is far from zero.

I think the velocity field is still developing. You should imagine a velocity and pressure field that is progressing from inlet to outlet while iterating from iteration 0. Just like opening a valve. So to me it looks like the velocity field has not been developed up until your outlet = my first guess. Of maybe your outlet is completely blocked by artificial walls. Could be anything. Impossible to say as long as your imbalance is way off.

So: create a plot where you monitor the imbalances of mass & momentum. These should all go to within 5%. At least. Only then look to residuals. Otherwise these are completely meaningless.

Now look at the velocity field of your calculation and see if it makes sense. If not, start from scratch and as simple as possible. Don't try to hit the roof in one go!:

1) Calculation 1: 1 m/s air at inlet. See if you can get this right completely.
2) Restart calculation 1 with new settings: 10 m/s air at inlet. See if you can get this right completely.
3) Restart calculation 2 with new settings: 10 m/s air at inlet and 10% 10 water. See if you can get this right completely.

And then progress existing calculations with increasing complexity. Higher velocities, inhomogeneous models, Total energy, etc. And ask your superviser to take a closer look.
Gert-Jan is offline   Reply With Quote

Old   April 5, 2018, 18:37
Default
  #15
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,645
Rep Power: 130
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your problems are more fundamental than rising residuals after 890 iterations. For instance you are modelling an inherently transient flow with a steady state model. It is never going to work as you currently have it set up.

To get straight to the point: You appear to be a beginner at CFD with very limited resources (student license, 500k nodes) attempting a simulation which is a big task for an experienced CFD person with access to a supercomputer. To put it bluntly, you are not going to successfully complete this simulation.

That is why I asked the question "why are you doing this?".

If the answer is because my professor told me to - then your professor set an impossible task and you need to get your professor to be realistic.

If the answer is because I thought it would be interesting to simulate it - then you should change it to a more reasonable simulation, for instance reducing the spray pressure/speed as Gert-Jan suggests would be a good approach.

If the answer is because it is part of a machine I am designing which uses this device to spray fluid - then you should look at either the literature for experimental/empirical work on high pressure sprays and estimate the spray performance from there, or use models like the lagrangian spray model in CFD to model the spray process.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 16, 2018, 04:26
Default
  #16
Member
 
Join Date: Mar 2018
Posts: 30
Rep Power: 5
Spray_Ansys is on a distinguished road
Thank you everybody for the inputs and answers.
I've just wanted to inform you, that the calculation and simulation finally came to an end and the result is satisfying. There were ~300 Iteration needed and finished after 30min.

Thanks to some changes in heat transfer, turbulence model and fluid model the wished solution came out. I'm now very happy that I reached the end of this task and can move forward in my bachelor thesis.

With this words I want to finish this thread. If someone has some more questions to my solution, please feel free to contact me via PM.

Thank you and kind regards
Spray_Ansys
Attached Images
File Type: jpg CFDonline_00.jpg (108.7 KB, 18 views)
File Type: jpg CFDonline_04.jpg (48.2 KB, 23 views)
File Type: jpg CFDonline_01.jpg (35.9 KB, 19 views)
Spray_Ansys is offline   Reply With Quote

Reply

Tags
ansys, cfx, convergance, residual, spray

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Simulation of ball-valve opening w.r.t to varying inlet pressure wasim_03 Main CFD Forum 1 January 6, 2018 12:40
outlet pressure Boundary settings -velocity streamline under ambient temp.conditions Vishnu_bharathi CFX 12 November 21, 2017 06:56
spray injection mmacrb FLUENT 0 January 10, 2007 04:57
Gas pressure question Dan Moskal Main CFD Forum 0 October 24, 2002 22:02


All times are GMT -4. The time now is 22:45.