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

vof fluid sloshing dispersed fluid and continuous fluid

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 26, 2016, 01:21
Exclamation vof fluid sloshing dispersed fluid and continuous fluid
  #1
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
hello

i have done simulation of water sloshing in rectangular tank, in empty space of water tank there is air,
i have selected for water as dispersed fluid with mean diameter of 0.05 [m] and air as continuous fluid,

i am showing two images one is simulated image and other is experimental,

my question is in both experimental and Ansys simulated videos motion are similar, but in Ansys i am not getting bubble/drops/spray formation as same as experiment (shown in image please seen)
i guess i need to change physics setting of dispersed fluid diameter, or is there anything i need to change, do can i put air as dispersed fluid

help me

thank you
Attached Images
File Type: jpg Capture.JPG (25.7 KB, 54 views)
File Type: jpg experomental image.JPG (28.3 KB, 49 views)
navi is offline   Reply With Quote

Old   August 26, 2016, 07:04
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,539
Rep Power: 128
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
I think you need to do some research on droplet formation. There is plenty of literature on it, and it is important background information what you need to know before you simulate it.

You will need:
1) A surface tension model
2) A finer mesh
3) A very small time step (don't guess this, use adaptive time stepping to home in on 3-5 coeff loops per iteration).
4) Plenty of computer time. It will be a big simulation.
5) Most simulations of this sort of thing use a homogenous free surface model. You don't need to set droplet diameters for this model as it models the formation of the droplets itself.
ghorrocks is offline   Reply With Quote

Old   August 26, 2016, 07:23
Default
  #3
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
Yeah thanks. I have seen so many papers but i dint get any details about mean diameter for dispersed fluid

If i don't give diameter. Then i should give both as continuous fluid.
And
I am in fine mesh tetrahedral .i know i cant ask mesh detail in cfx form. But this mesh is important for vof modeling
Can i use for this simulation an hexahedral mesh pr tetrahedral mesh. Due to large time of simulation
navi is offline   Reply With Quote

Old   August 26, 2016, 07:42
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,539
Rep Power: 128
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:
Then i should give both as continuous fluid.
Correct.

Quote:
I am in fine mesh tetrahedral
Surface tension is highly sensitive to mesh quality. You will want to use hex meshes with 1:1 aspect ratio if at all possible.
ghorrocks is offline   Reply With Quote

Old   August 26, 2016, 07:46
Default
  #5
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
Thanks. Ill simulate it
navi is offline   Reply With Quote

Old   August 29, 2016, 02:40
Question
  #6
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
hello glenn

I have changed hex mesh with aspect ratio details i have given in attachment,

and I have used surface tension model > in that there is volume fraction smoothening type is there , i searched about that I didn't get THEORY about that,and what to select in that,
similar in solver setting , there is initial volume fraction smoothening is automatically selected (volume weighted) , what is this in surface tension model, now i have put for simulation ill check ill get water droplet or not,
check my setting given right to get droplet
Attached Images
File Type: jpg Capture.JPG (65.1 KB, 36 views)
File Type: jpg df.JPG (37.3 KB, 30 views)
File Type: jpg fhj.JPG (63.2 KB, 28 views)
File Type: jpg DOMOAIN.JPG (120.6 KB, 36 views)
File Type: jpg ASPECT RATIO.JPG (25.2 KB, 27 views)
navi is offline   Reply With Quote

Old   August 29, 2016, 07:37
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,539
Rep Power: 128
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
1) Your mesh has some wonky bits in it. You want it to be perfect hexas. Use mapped mesh faces to make sure they are perfect hexas.

2) You have shown a few of the free surface modelling options. Surface tension models are very sensitive to some of these parameters and often you can do better than the defaults. But exactly what option works for you will depend on many factors. So I recommend you try all the options and see which ones work for you. Do a short benchmark simulation to test it and script it up so you can run lots of options quickly. Then you can find for yourself which options work (and don't work) in your case.
ghorrocks is offline   Reply With Quote

Old   August 29, 2016, 07:57
Unhappy
  #8
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
1) You have shown a few of the free surface modelling options. Surface tension models are very sensitive to some of these parameters and often you can do better than the defaults. But exactly what option works for you will depend on many factors. So I recommend you try all the options and see which ones work for you. Do a short benchmark simulation to test it and script it up so you can run lots of options quickly. Then you can find for yourself which options work (and don't work) in your case.

from your experience any suggestion to get droplets by changing free surface model, shown in initial message in this thread,,

navi is offline   Reply With Quote

Old   August 29, 2016, 08:01
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,539
Rep Power: 128
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
My posts #2 and #7 list what you need to look at.
ghorrocks is offline   Reply With Quote

Old   August 31, 2016, 01:25
Default no droplets
  #10
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
hey,

i tried lot to get droplets, but result is still negative,

i want to know that do really cfx Ansys tool , in vof model do we get droplets like experimental type exactly.
i tried everything using continuous fluid for both fluid, with surface tension model,
Attached Images
File Type: jpg Capture.JPG (25.7 KB, 15 views)
File Type: jpg experomental image.JPG (28.3 KB, 11 views)
navi is offline   Reply With Quote

Old   August 31, 2016, 02:15
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,539
Rep Power: 128
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
Have you drawn isosurfaces of volume fraction = 0.5?

Also if you could describe what you have tried that would help. I have already explained several times what you need to get this working but I cannot be more specific until you explain what you have tried - in enough detail that we can comment on it.
ghorrocks is offline   Reply With Quote

Old   August 31, 2016, 02:27
Default
  #12
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
yeah i tried isosurface, ill take a clip image all what i did in cfx outline tree, with expressions few min
navi is offline   Reply With Quote

Old   August 31, 2016, 02:40
Default all details of outline tree
  #13
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
i need to get droplets like experimental image, but i am not get droplet when fluid hits wall, other than droplet movement fo fluid is same as experimental

just check my setting in outline tree,
i changed for different simulation the relaxation factor, and volume fraction smoothening type (laplacian and volume-weighted both i tried)
Attached Images
File Type: jpg experomental image.JPG (28.3 KB, 14 views)
File Type: jpg air fluid details.JPG (122.3 KB, 17 views)
File Type: jpg Capture.JPG (58.8 KB, 13 views)
File Type: jpg df.JPG (44.3 KB, 14 views)
File Type: jpg expressions.JPG (22.8 KB, 15 views)
navi is offline   Reply With Quote

Old   August 31, 2016, 02:42
Default
  #14
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
other images of cfx pre setting
Attached Images
File Type: jpg nw.JPG (71.3 KB, 14 views)
File Type: jpg mesh details.JPG (143.4 KB, 19 views)
File Type: jpg water fluid details.JPG (121.2 KB, 12 views)
File Type: jpg fluid models.JPG (65.9 KB, 11 views)
File Type: jpg sq.JPG (78.0 KB, 11 views)
navi is offline   Reply With Quote

Old   August 31, 2016, 09:20
Default
  #15
Senior Member
 
urosgrivc
Join Date: Dec 2015
Location: Slovenija
Posts: 363
Rep Power: 8
urosgrivc is on a distinguished road
Hi

I have a question: Is mesh addoption appropriate for cases like this? or is extra computational effort (extra nodes in the mesh and time spent to refine the mesh) not worth the extra resolution.

-Maybe even to obtain the same amount of nodes but higher resolution where is needed (gas-liquid border)

-Mesh adoption could be done where fluid volume fraction has some value (or is between two walues)

-I imagine that it would look and work similar to a cut cell mesh, but would be able to run within cfx for simple geometries like this, as cutcell is not suported.

Well that is the idea anyway
just a thought
It seems an interesting case to me
urosgrivc is offline   Reply With Quote

Old   August 31, 2016, 09:45
Default Hey grvic
  #16
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
Its interesting only
But
I dont get about mesh adoption.
navi is offline   Reply With Quote

Old   August 31, 2016, 19:56
Default
  #17
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,539
Rep Power: 128
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
Surface tension models are extremely sensitive to mesh quality. You get a significant error with elements with an aspect ratio of just 1.2. So in my experience the mesh adaption methods used in CFX cannot keep the mesh quality high enough to remain accurate.

Fluent has a hanging node mesh refinement which keeps mesh quality high. I have used this in fluent and had good results. But to make it dynamically track interfaces is not easy It took me several months of work to get the mesh refinement to dynamically track the interface.

So unless you want to spend several months developing a hanging node dynamic mesh refinement algorithm in Fluent, then just use a 1:1 aspect ratio hex mesh with no mesh refinement.

I have seen no comment that naveen has done sensitivity studies of mesh resolution, time step or convergence. He is wasting his time looking at other things until he has checked these basic parameters.

Also I note you have set a maximum of 4 coeff loops per iteration. That appears unnecessarily restrictive. It should be 10 and you should use adaptive time stepping homing in on 3-5 coeff loops per iteration.
ghorrocks is offline   Reply With Quote

Old   September 1, 2016, 01:21
Default hey glenn
  #18
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
actually, i need to learn more about mesh resolution ill do that thanks,
as i am doing in cfx, and i dint try in fluent.

and can you tell me exactly in mesh what to study , because i am new to mesh ansys everything
navi is offline   Reply With Quote

Old   September 1, 2016, 02:19
Default
  #19
Member
 
naveen kumar s
Join Date: Aug 2016
Location: india, bengalore
Posts: 51
Rep Power: 6
navi is on a distinguished road
hey
i need to get this job done ASAP, can u tell me just procedure to mesh and physics, and ill see steps and i can learn easily, i have a very short dead line
navi is offline   Reply With Quote

Old   September 1, 2016, 07:30
Default
  #20
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 16,539
Rep Power: 128
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
One key factor is to ensure that the tunable parameters of your model are set correctly. For most models they are the mesh density, converge tolerance and time step size (if transient).

The time step size is the simplest - just use adaptive time stepping homing in on 3-5 coeff loops per iteration and it will automatically find the correct time step. If you manually set the time step you will need to do sensitivity studies on time step size as well.

You will need to do sensitivity studies on mesh density and convergence tolerance. The procedure is:
1) Run your simulation with the current settings
2) If doing mesh sensitivity then remesh with the element edge length halved (so 8 times the element count in 3D).
3) Run your simulation on the new mesh.
4) Compared the simulation results of 1) and 3) using a parameter of interest to you. It could be pressure loss, lift, drag, flow rate... what ever is important to your analysis.
5) If the two simulations give values of the parameter closer than an error tolerance you are happy to live with then you are finished and you have found the mesh density your require.
6) If the two simulations give different results you need to halve the element edge length again and go to step 3 - repeat this process, refining the mesh until you converge within a tolerance you are happy to live with.

For convergence tolerance also do a sensitivity study, but start with your current residuals tolerance, and do 10 times tighter for the next step. Keep refining convergence tolerance by a factor of 10 until it converges.

You should now have found a time step, mesh and convergence tolerance which you have shown to be suitable for your application. You can now proceed knowing that you have done some basic accuracy checks on your simulation.

There are more sophisticated ways of doing this with converge much faster. As mesh refinement gets very expensive very quickly this becomes important for real world cases (for instance: http://journaltool.asme.org/Template...umAccuracy.pdf). But I would not use these techniques until you can manage the simple process I have described.
ghorrocks is offline   Reply With Quote

Reply

Tags
dairy equipment, dispersed fluid, sloshing, sloshingtank3d, spray dryer, vof

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
Wrong flow in ratating domain problem Sanyo CFX 17 August 15, 2015 07:20
Overflow Error in Multiphase Modelling with Two Continuous Fluids ashtonJ CFX 6 August 11, 2014 15:32
Multiphase flow with two continuous fluids and one dispersed fluid ashtonJ CFX 5 July 25, 2014 07:31
How to choose the mean diameter value for dispersed fluid? creddy_trddc CFX 1 October 30, 2011 05:30
air bubble is disappear increasing time using vof xujjun CFX 9 June 9, 2009 08:59


All times are GMT -4. The time now is 06:24.