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

sprayFoam

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

Like Tree1Likes
  • 1 Post By Akuji

Reply
 
LinkBack Thread Tools Display Modes
Old   January 25, 2013, 04:34
Default sprayFoam
  #1
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Hello!

I need a solver to visualized a liquid spray. As I see in tutorials of OF, one of solvers I can use is sprayFoam (I need only first 2 steps: spray breakup and spray tracking).
At 1st I made a tutorial aachenBomb. the results are ok: filed of velocity and pressure seem to be real, but when I try to see particles [foamToVtk and then load sprayCloud], paraview closed with "Segmentation fault".

UPD. On another machine paraview work ok,but I don't see any particles .It seems there are no particles.

Does anyone know what do I do wrong?

Maybe someone has a similar task and can help me.

Another question: I found an information about CFDEM and LIGGGHTS. As I understand it is possible to solve my problem using it. But I didn't find any information of their tutorials. Maybe I compiled it not correct, but I didn't see any results after making tutorial cfdemSolverPiso/settlingTestMPI.
Maybe someone can give me more information about it.

Last edited by Akuji; January 25, 2013 at 04:58.
Akuji is offline   Reply With Quote

Old   January 25, 2013, 13:54
Default
  #2
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
Since you mentioned sprayFoam I'm assuming your are using OF 2.1.x. You should be able to just load the defaultCloud in ParaFoam and then extract it using the extractBlock filter. Try that and see what happens.
mturcios777 is offline   Reply With Quote

Old   January 28, 2013, 09:37
Default
  #3
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Quote:
Originally Posted by mturcios777 View Post
Since you mentioned sprayFoam I'm assuming your are using OF 2.1.x. You should be able to just load the defaultCloud in ParaFoam and then extract it using the extractBlock filter. Try that and see what happens.
Thanks for advance, mturcios777. I use OF-2.1.0 you were right.
About paraview: I made as you sad. Load defaultCloud (hope you mean spray.foam), then I used extractBlock filter. After that I choose in pipelan browser interanlMesh, but after it I can load velocity field and pressure field on the same picture together. But I didn't find particles.

I copy from another directory ParticleTrackProperties in constant/ and use particleTracks. After that I have a directory VTK, inside it - particleTracks.vtk
This file I load in paraview, then use Glyph filter - visible spheres. The results of my operation I attach. But I have a doubt - are they right? For my opinion tracks of particles are not right.
Velocity field and pressure field are ok.spray.jpg
3_003.jpg
Akuji is offline   Reply With Quote

Old   January 28, 2013, 13:28
Default
  #4
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
Hi Akuji,

What are you scaling the glyph diameter by? Sometimes the distribution can look misleading because of a uniform diameter. Also, what does the temperature look like?
mturcios777 is offline   Reply With Quote

Old   January 28, 2013, 15:10
Default evaporating_drops.ccl
  #5
New Member
 
Alime Cengiz
Join Date: Jan 2013
Posts: 8
Rep Power: 4
cngz is on a distinguished road
Hi,
It is not related to spray foam but could you please send the tutorial file "evaporating_drops.ccl" It is for "Spray Dryer" tutorial? I need it so badly!
alimecngz@gmail.com
cngz is offline   Reply With Quote

Old   January 28, 2013, 15:14
Default
  #6
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
I don't have this tutorial case, I'm not sure what version of OpenFOAM it belongs to. Sorry
mturcios777 is offline   Reply With Quote

Old   January 28, 2013, 15:17
Default
  #7
New Member
 
Alime Cengiz
Join Date: Jan 2013
Posts: 8
Rep Power: 4
cngz is on a distinguished road
it belongs to ANSYS CFX 13. Thanks anyway
cngz is offline   Reply With Quote

Old   January 29, 2013, 06:40
Default
  #8
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Quote:
Originally Posted by mturcios777 View Post
Hi Akuji,

What are you scaling the glyph diameter by? Sometimes the distribution can look misleading because of a uniform diameter. Also, what does the temperature look like?
I use scale mode - scalar. Set scale factor - automatically.
About temperature: at time 0.0015 there is no field of temp. Because I don't need a part of tutorial with combustion, I cut all times where there is no any injection of particles.
The diameter of scaling is 1 (r=0.5). If I choose smaller radius, image is the same, just particles look smaller.
Akuji is offline   Reply With Quote

Old   January 29, 2013, 14:17
Default
  #9
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
I know you can scale the particles to be proportional to their mean diameter. Is there any evaporation happening?
mturcios777 is offline   Reply With Quote

Old   February 8, 2013, 05:05
Default
  #10
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Hello!

About evaporation - really I don't know. The last time when parcels are added is t=0.0125:

Time = 0.00125


Solving cloud sprayCloud

--> Cloud: sprayCloud
Added 56 new parcels

Cloud: sprayCloud
Current number of parcels = 18944
Current mass in system = 4.12019e-07
Linear momentum = (-1.64279e-07 -3.21616e-05 -3.42757e-08)
|Linear momentum| = 3.21621e-05
Linear kinetic energy = 0.0025296
Rotational kinetic energy = 0
Total number of parcels added = 123490
Total mass introduced = 5.99999e-06
Parcel fates:
- escape = 0, 0
- stick = 0, 0
Mass transfer phase change = 5.58798e-06
D32 (mu) = 6.71635
Liquid penetration 95% mass (m) = 0.0193151

As I understand, evaporation exist, because current number of parcels if 18 944, and total number of parcels added is 123 490.
Another step I did, i finally understand how to use vtk file for my time. The spray seems to be real.
Question I have: how to see the distribution of parcels according to their diameter? D32 is 6.7e-6m (am I right?). So, to see the particles I use glyph type sphere, radius = 1, scale mode = 6.7e-6. And my particles have one size and one color.
Attached Images
File Type: jpg 1111.jpg (21.3 KB, 91 views)
Akuji is offline   Reply With Quote

Old   February 8, 2013, 13:36
Default
  #11
Senior Member
 
mturcios777's Avatar
 
Marco A. Turcios
Join Date: Mar 2009
Location: Vancouver, BC, Canada
Posts: 727
Rep Power: 18
mturcios777 will become famous soon enough
I would also plot the mass fraction of what is evaporating. If all the particles are constant diameter, then the distribution looks feasible, since parcels break up as we leave the nozzle, increasing the number of parcels while evaporation reduces the number.

I would also plot the mass fraction of the species that is evaporating in the droplets.
mturcios777 is offline   Reply With Quote

Old   March 5, 2013, 07:52
Default
  #12
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Well, after some weeks of solving I still have questions.

1. How does sprayFoam calculate D32? According to my calculation I have particles size 1.3mm, and foam calculate as 21581.9 (*10^-6 am I right?).

2. I don't need an evaporation, combustion, chemiacl reactions and other parts. I am interested only in the particle size, path and the particle interaction and particle-to-wall interactions. I turn off evaporation, combustion and etc., change chem.inp file but still have dependence of Temperature:
Code:
DILUPBiCG:  Solving for hs, Initial residual = 0.000893686, Final residual = 1.45528e-10, No Iterations 1
T gas min/max   = 252.514, 320.275
Variation of temperature is too much.


So, example of output in my terminal:
Code:
Cloud: sprayCloud
    Current number of parcels       = 17136
    Current mass in system          = 0.171842
    Linear momentum                 = (7.11313e-06 1.24111e-05 -0.218256)
   |Linear momentum|                = 0.218256
    Linear kinetic energy           = 5.49125
    Rotational kinetic energy       = 0
    Total number of parcels added   = 17136
    Total mass introduced           = 0.171842
    Parcel fate (number, mass)
      - escape                      = 0, 0
      - stick                       = 0, 0
    Mass transfer phase change      = 0
    D10, D32, Dmax (mu)             = 2027.54, 21581.9, 99996.5
    Liquid penetration 95% mass (m) = 0.076189

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 0.000416571, Final residual = 5.39093e-11, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.00125617, Final residual = 1.83274e-10, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.000726465, Final residual = 5.80187e-11, No Iterations 1
DILUPBiCG:  Solving for H2O, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for hs, Initial residual = 0.000893686, Final residual = 1.45528e-10, No Iterations 1
T gas min/max   = 252.514, 320.275
DICPCG:  Solving for p, Initial residual = 0.00118179, Final residual = 2.15544e-08, No Iterations 1
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 4.94038e-11, global = 1.54421e-14, cumulative = 1.204e-08
DICPCG:  Solving for p, Initial residual = 2.68447e-07, Final residual = 2.68447e-07, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 6.18547e-10, global = 4.59799e-15, cumulative = 1.204e-08
DILUPBiCG:  Solving for omega, Initial residual = 3.89693e-07, Final residual = 3.89693e-07, No Iterations 0
DILUPBiCG:  Solving for k, Initial residual = 1.07217e-05, Final residual = 2.39036e-12, No Iterations 1
I have no idea what is wrong (well, maybe I choose wrong solver?)

If you have an idea or any free time, please, see my attached files: I think there are some mistakes too.
Attached Images
File Type: jpg problem.jpg (12.7 KB, 56 views)
Attached Files
File Type: txt chem.txt (39 Bytes, 15 views)
File Type: gz constant.tar.gz (2.4 KB, 20 views)
Akuji is offline   Reply With Quote

Old   March 5, 2013, 09:54
Default
  #13
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
Quote:
Originally Posted by Akuji View Post
Well, after some weeks of solving I still have questions.

1. How does sprayFoam calculate D32? According to my calculation I have particles size 1.3mm, and foam calculate as 21581.9 (*10^-6 am I right?).
http://foam.sourceforge.net/docs/cpp/a05046_source.html
Check the Dij-function, D32 = Dij(3,2)

The biggest droplets are around 0.1m...which i think probably is a mistake.

Quote:
Originally Posted by Akuji View Post

2. I don't need an evaporation, combustion, chemiacl reactions and other parts. I am interested only in the particle size, path and the particle interaction and particle-to-wall interactions. I turn off evaporation, combustion and etc., change chem.inp file but still have dependence of Temperature:
Code:
DILUPBiCG:  Solving for hs, Initial residual = 0.000893686, Final residual = 1.45528e-10, No Iterations 1
T gas min/max   = 252.514, 320.275
Variation of temperature is too much.


So, example of output in my terminal:
Code:
Cloud: sprayCloud
    Current number of parcels       = 17136
    Current mass in system          = 0.171842
    Linear momentum                 = (7.11313e-06 1.24111e-05 -0.218256)
   |Linear momentum|                = 0.218256
    Linear kinetic energy           = 5.49125
    Rotational kinetic energy       = 0
    Total number of parcels added   = 17136
    Total mass introduced           = 0.171842
    Parcel fate (number, mass)
      - escape                      = 0, 0
      - stick                       = 0, 0
    Mass transfer phase change      = 0
    D10, D32, Dmax (mu)             = 2027.54, 21581.9, 99996.5
    Liquid penetration 95% mass (m) = 0.076189

diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for Ux, Initial residual = 0.000416571, Final residual = 5.39093e-11, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.00125617, Final residual = 1.83274e-10, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.000726465, Final residual = 5.80187e-11, No Iterations 1
DILUPBiCG:  Solving for H2O, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG:  Solving for hs, Initial residual = 0.000893686, Final residual = 1.45528e-10, No Iterations 1
T gas min/max   = 252.514, 320.275
DICPCG:  Solving for p, Initial residual = 0.00118179, Final residual = 2.15544e-08, No Iterations 1
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 4.94038e-11, global = 1.54421e-14, cumulative = 1.204e-08
DICPCG:  Solving for p, Initial residual = 2.68447e-07, Final residual = 2.68447e-07, No Iterations 0
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 6.18547e-10, global = 4.59799e-15, cumulative = 1.204e-08
DILUPBiCG:  Solving for omega, Initial residual = 3.89693e-07, Final residual = 3.89693e-07, No Iterations 0
DILUPBiCG:  Solving for k, Initial residual = 1.07217e-05, Final residual = 2.39036e-12, No Iterations 1
I have no idea what is wrong (well, maybe I choose wrong solver?)

If you have an idea or any free time, please, see my attached files: I think there are some mistakes too.

How much time have elapsed and how much water are you supposed to inject, because that looks like quite alot. (remember that injected mass is in kg)
niklas is offline   Reply With Quote

Old   March 5, 2013, 09:58
Default
  #14
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 20
niklas will become famous soon enoughniklas will become famous soon enough
remember also that length is in meters, not millimeters
niklas is offline   Reply With Quote

Old   March 9, 2013, 06:30
Default
  #15
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
niklas,

thank you for your help. I find Dji in KinematicCloudI.H, but didn't understand how it calculates (my c++ knowledge is very bad). But I see then more I have mass flow then less diametr my particles have.
About Dmax: I don't know exactly how solver works, but in my work I have drops of water. They interract between themselves: can divide or couple for more smaller or larger particle. Dmax=0.1m is probably puddle on the floor or on the wall (it is my explanation why it is so large).

I reviewed my b.c. and my mass flow is ok (I plan to inject 10 kg/s from my nozzle). My mesh is in meters.
Akuji is offline   Reply With Quote

Old   March 18, 2013, 03:58
Default
  #16
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Hello again!

A added a Blob Atomization model for primary break-up, but have no difference with my previous effort.

Now I have a problem: when my particles reach disk they have absolutely elastic impact. They fly to the patch which from they fall. And for them it is not important that it is injection still work. In fluent I have very nice results for my room, but in OF there is no any spray dissemination

Any ideas?..

Last edited by Akuji; March 28, 2013 at 06:19.
Akuji is offline   Reply With Quote

Old   April 4, 2013, 09:54
Default
  #17
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Really sad, but particles just bounce between out-patch and disk-patch

Akuji is offline   Reply With Quote

Old   April 22, 2013, 11:59
Default
  #18
New Member
 
Vito Raso
Join Date: Apr 2013
Location: Bari(Italy)
Posts: 7
Rep Power: 4
Vito31388 is on a distinguished road
Hi Akuji, I don't understand how visualize in paraview particles in the spray cloud for aachen bomb tutorial; I've used foamToVTK to create VTK files but when I select spraycloud.vtk and I choose glyph,I don't see the particles.Can you explain me the procedure?
Vito31388 is offline   Reply With Quote

Old   April 22, 2013, 14:45
Default
  #19
Member
 
Arina
Join Date: Oct 2009
Location: Belarus
Posts: 76
Rep Power: 7
Akuji is on a distinguished road
Send a message via ICQ to Akuji
Quote:
Originally Posted by Vito31388 View Post
Hi Akuji, I don't understand how visualize in paraview particles in the spray cloud for aachen bomb tutorial; I've used foamToVTK to create VTK files but when I select spraycloud.vtk and I choose glyph,I don't see the particles.Can you explain me the procedure?
Hi, Vito!

In the example I load spraycloud.vtk, choose glyph: type - sphere and scale mode - scalar, then apply. If you still don't see particles, try to edit scalar factor: for example, use not 0.002 but 0.02 - you will see difference. And use for example time=11, not 0 or 1.
Good luck!
Vito31388 likes this.
Akuji 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
aachenBomb with sprayFOAM not working jenzkeller OpenFOAM Bugs 8 June 8, 2014 18:01
Incorrect introduced mass in sprayFoam? sushant OpenFOAM Running, Solving & CFD 15 May 29, 2014 21:17
sprayFoam crashes lukasfischer OpenFOAM Running, Solving & CFD 3 July 14, 2013 11:08
sprayFoam void fraction dkxls OpenFOAM 2 September 16, 2012 13:39
sprayFoam results depend on the type of chemistryReader (chemkinReader/foamChemistry arash1 OpenFOAM Running, Solving & CFD 1 April 2, 2012 12:47


All times are GMT -4. The time now is 15:52.