
[Sponsors] 
November 22, 2011, 00:23 
How to calculate freesurface distance,velocity,etc...

#1 
New Member
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 7 
Hi,
I'm triyng simulate droplet formation through a tjunction (using interFoam), but now i have to compute the average interdrop distance, drops velocity and their lenght. For the lenght i have found a temporary solution using paraFoam contour>clip>slice, for the plot alpha1 vs time I use probe in controlDict and for others measurements the sample utility but for the interdrop distance or drops velocity i have no idea. Thanks in advance. droplet.png 

November 22, 2011, 03:19 

#2 
Senior Member
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 790
Rep Power: 14 
Maybe you can sample the value of alpha1 over the centerline of the channel. Then you need to write a small script to process the [x, alpha1] data, but I suppose you get the point.


May 30, 2012, 06:22 

#3  
New Member
A Sharma
Join Date: Mar 2012
Location: Germany
Posts: 14
Rep Power: 6 
Hello OpenFoam User,
I am a new to openFoam and currently interested in simulating droplet formation through a T Junction. The image you posted for droplet formation looks really nice. It will be of great help if you can suggest me how to proceed with interFoam to study droplet formation. Sincerely, as Quote:


May 30, 2012, 20:50 

#4 
New Member
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 7 
yes, i have hardly worked on this and i'm happy that may be useful for someone.
what are your problems? boundary conditions, geometry, results analysis....? 

May 31, 2012, 03:04 

#5 
New Member
A Sharma
Join Date: Mar 2012
Location: Germany
Posts: 14
Rep Power: 6 
Hello deifobe,
Many thanks for your response. I am using the example "damBreak" to create my system. So I created a T Junction Geometry, uses the similar files for "system" as in the damBreak example (I hope they are correct for this). I think the major problem I get is in defining the boundary conditions for two phase flow. It will be of great help if you can explain how you have defined the boundary conditions for two inlets and one outlet or if possible you may give me a demo file for them. Thanks a lot, as 

June 5, 2012, 09:38 

#7 
New Member
A Sharma
Join Date: Mar 2012
Location: Germany
Posts: 14
Rep Power: 6 
Hello,
Thanks you very much for such a useful file. I was trying to improve the geometry but I stuck with a problem. For Eg: If I try to change some variables of your file : InletOil > InletA InletWater > InletB, I make the changes at the following places : 1) blockMeshDict 2) alpha1.org 3) alpha 4) p_rgh 5) U and then I tried : blockMesh setFields interFoam, simulation starts fine but min(alpha1) in my simulation goes negative. And I observe something different in paraFoam. What is the expected problem or some important point I am missing ? Please have a look at the attached file. Thanking You, Sincerely, as 

June 5, 2012, 09:55 

#8 
New Member
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 7 
Hi guy,
it's ok that min(alpha1) is negative, what you observe different in paraFoam? Please, post a n image of your result. 

June 5, 2012, 10:10 

#9 
New Member
A Sharma
Join Date: Mar 2012
Location: Germany
Posts: 14
Rep Power: 6 
Hello,
Here is the Image after first time step. I am surprised as in your case minAlpha is approx zero (even negative but almost zero). And, just by changing the variable names, I get different values (negative that too increases with time). I think I am doing some blunder while defining the initial conditions. Thanx as 

June 5, 2012, 10:45 

#10 
New Member
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 7 
the inlet in which you set alpha1=1
(from alpha1 file: inletA { type fixedValue; value uniform 1; }) is the the inlet of the dispersed (droplet) phase (e.g. water). Then you are wrong in the blockMeshDict file, you must exchange in this file inletA with inletB, to understand this you can draw the geometry on a paper with vertices numbers. 

June 11, 2012, 12:53 
Small Time Step

#11  
New Member
A Sharma
Join Date: Mar 2012
Location: Germany
Posts: 14
Rep Power: 6 
Hello deifobe,
Thanks for pointing out my mistake. I used your file to create little bit complex setup (as shown in fig. attached). In this case when I run the same, deltaT becomes very small of the order of 1e11. Is this usual or problematic ? Please let me know if you have encountered this type of problem. I expect this due to mesh I created, which effects the Courant number. It will be be great help if you can suggest me how to solve this problem ? Many thanks for your help. A. Sharma Quote:


April 20, 2013, 13:04 

#12 
Member
Join Date: Mar 2013
Posts: 94
Rep Power: 5 
Hi to all
I have a similar problem. My geometry is an horizontal pipe completely filled with liquid. At initial time the air can enter into the pipe and form a bubble that move forward into the pipe. I want to calculate the velocity and the position of the front of the bubbles over pipe channel length and the height of the bubble over time. You have any suggestion? Thanks a lot 

April 20, 2013, 15:02 

#13 
New Member
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 7 
Hello,
you can use the probes for U and alpha1 in controlDict file choosing a line that passes through the middle of your channel. After, you can elaborate the output probe file for alpha1 by octave or matlab to find the positions of the front of the bubble vs time finding the points in which the value of alpha1 is about 1 (has a maximum). I hope this will help. 

April 21, 2013, 17:57 

#14 
Member
Join Date: Mar 2013
Posts: 94
Rep Power: 5 
thank you for your reply.
I already completed simulations so I look for a way to postprocess without restart their. Moreover I don't know the position of the bubble front so I don't know where place probes... 

April 23, 2013, 06:35 

#15 
New Member
Lidia
Join Date: Oct 2011
Posts: 13
Rep Power: 7 
You can use the sample utility but you will obtain, the values of alpha1 and U split in time directories, in my opinion in this manner is more complicated to extract the data that you need.
This is an example of sampleDict: interpolationScheme cell; setFormat gnuplot; sets ( centerPatch { type uniform; axis xyz; //line in the middle of horizontal channel start (0.00046 5e05 25e06); end (0.00041 5e05 25e06); nPoints 100; } ); surfaces (); fields ( alpha1 ); I suggest you to use the probes choosing a set of equally spaced points on the line in the middle of horizontal channel. 

April 23, 2013, 07:10 

#16 
Member
Join Date: Mar 2013
Posts: 94
Rep Power: 5 
thank you,I'll try it. but in this way I calculate alpha and U in middle of channel?I need U of the front of bubble that isn't in pipeline center.
I tried this procedure: contour of alpha=0.5 slice normal to x at 0,0,0 slice normal to y at 0,0.0175,0 plot selection over time the result are ok but the problem is the follow: the front bubble is not at a constant y but vary between 0.015 and 0.0175 so I must view manually when the y bubble front change and merge two graphics. After set contour of alpha=0.5 there is a way to choose the minimum value of a coordinates (z in my case)? In this way would be all automatic 

April 23, 2013, 19:56 

#17  
Assistant Moderator
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,987
Rep Power: 41 
Quote:
__________________
Note: I don't use "Friend"feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Thermocapillary free surface flow  zakifoam  OpenFOAM Running, Solving & CFD  10  December 12, 2016 12:44 
Submarine Free Surface  samwh  CFX  7  August 30, 2009 07:14 
Multiphase flow. Dispersed and free surface model  Luis  CFX  8  May 29, 2007 18:13 
Equilibrium of a free surface under surface tensio  Ryan  Main CFD Forum  1  August 7, 2001 16:14 
Modeling Free Surface Flows  Elliot Schwartz  Main CFD Forum  5  August 25, 1998 21:03 