|
[Sponsors] |
![]() |
![]() |
#1 |
New Member
Thomas
Join Date: Mar 2018
Location: Germany
Posts: 18
Rep Power: 8 ![]() |
Hi there,
I am trying to extract the Volume of entrained air by an impinging jet during the filling process of liquids. I inserted an Isovolume (Volume Fraction of Liquid < 0.65) which results in an Isovolume with two bodies (One for the Air above the Free Surface and One for the Bubble below the Free Surface). I am able to quantify the volume of this Isovolume, but I have difficulties to seperate the volumes of the two bodies. How can i extract the volume of only one of the bodies? |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Good point. This appears to be something missed in CFD-Post - that is, you can only define the domain and element type it makes a isovolume from. You cannot define it gets it from some other volume (such as another isovolume).
To work around this, define a new variable, equal to the volume fraction, but using a "if" statement to set the variable to zero on one side of the the free surface. Then you can do a isovolume of the new variable and get what you want.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
![]() |
#3 | |
New Member
Thomas
Join Date: Mar 2018
Location: Germany
Posts: 18
Rep Power: 8 ![]() |
Quote:
thanks for the reply, but I am not sure how to realize your suggestion. My isovolume as of right now appears as following: ![]() I implemented the expression if(water.Conservative Volume Fraction.Beta<=0.65,1,0) but I have no success in seperating the two volumes. Thanks in advance for any further advice! |
||
![]() |
![]() |
![]() |
![]() |
#4 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
you should create a variable that is equal to your expression. Then you can create an isovolume using that variable.
|
|
![]() |
![]() |
![]() |
![]() |
#5 |
New Member
Thomas
Join Date: Mar 2018
Location: Germany
Posts: 18
Rep Power: 8 ![]() |
When i use the following expression
if(water.Conservative Volume Fraction.Beta<=0.65,1,0) as a variable, and create an isovolume for the variable at value = 0 i get the following Volume. ![]() I tried all options for the isovolume (at value, below value etc.) but could not get the right isovolume As i understand the expression, the variable will take the value 1 for all parts in the domain where the volume fraction of the liquid is less than 0.65, and the value 0 otherwise. This will not seperate the two volumes to result in only the volume inside of the liquid. How should i write the expression? |
|
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,885
Rep Power: 27 ![]() |
You could include the Y coordinate.
You should determine the Y value that lies between the bubble and the free surface. Say this is Y1. Then you should multiply the volume fraction with step(-Y1). This will be zero above Y1 and 1 below Y1. In this way you can separate both volumes. Certainly this won't work if the bubble is much more complicated in shape, but here it should work. Alternatively, you can include X and Y. |
|
![]() |
![]() |
![]() |
![]() |
#7 |
New Member
Thomas
Join Date: Mar 2018
Location: Germany
Posts: 18
Rep Power: 8 ![]() |
Yeah, I was thinking about this, but as I want to track the bubble volume during the whole transient simulation this won`t help for more complicated bubble types.
I also started with image processing of the transient video file with matlab but think a solution within ANSYS CFX Post will be more accurate. EDIT: I used the wrong variable with water.Conservative Volume Fraction.Beta, I should have used water.Conservative Volume Fraction With the inclusion of the Y-Coordinate in my expression I am able to get the Volume of the bubble. But I will not be able to track the bubble size during the whole transient simulation with this method. Last edited by dickes; September 14, 2018 at 08:09. |
|
![]() |
![]() |
![]() |
![]() |
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,816
Rep Power: 144 ![]() ![]() ![]() ![]() |
Yes, sound like you need a more sophisticated technique for tracking this over the whole simulation. Look at blob detection algorithms from image processing techniques, these may have some useful ideas. There are some nice libraries in python to do this which I have used often, such as opencv, scikit (https://scikit-image.org/) and mahotas. Interfacing these with CFX to run automatically will be an interesting challenge
![]()
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Using CFD Post for OpenFoam results | Karpfen | OpenFOAM Post-Processing | 3 | January 19, 2018 08:48 |
On the CFD market and trends | sbaffini | Main CFD Forum | 14 | June 13, 2017 11:48 |
Post-processing star ccm+ results in Ansys CFD Post | sidharath | STAR-CCM+ | 4 | April 10, 2017 11:49 |
Post processing in CFD Post or Fluent. | Blobs | OpenFOAM Post-Processing | 2 | June 26, 2016 07:23 |
CFD Online Celebrates 20 Years Online | jola | Site News & Announcements | 22 | January 31, 2015 00:30 |