
[Sponsors] 
November 3, 2021, 09:38 
CFDPost evaluation

#1 
New Member
Lukas
Join Date: Sep 2021
Posts: 9
Rep Power: 2 
Hello,
I want to quantify the zone under the isosurface shown in the picture. Therefore I calculate volume and length. Is there a way of doing it in CFDPost? For now, I'm exporting the surface and calculate the result in MATLAB. But as I want to automate the process, the sweetest option would be to do it in CFDPost. Thanks in advance, Lukas 

November 13, 2021, 07:09 

#2 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,388
Rep Power: 21 
You can create a volume from an isosurface. Then the elements below, at or above can be included. This volume can be quantified using an expression.
Remember that the isosurface is an interpolation in space. The volume method includes whole elements which will not align with the isosurface. So, the method will deviate from what you probably will determine in MATLAB. This should not be a problem as long as you know what you are doing. What also helps is to reduce local mesh size. 

November 13, 2021, 07:55 

#3  
New Member
Lukas
Join Date: Sep 2021
Posts: 9
Rep Power: 2 
Quote:
First of all thanks for your reply. What kind of expression do I need? What should it look like? 

November 13, 2021, 08:43 

#4 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,388
Rep Power: 21 
You can use the function calculator. Look for the function volume and the location i.e. the volume as covered by your isosurface.
By pressing apply, you will find the volume. If you tick on "Show equivalant expression", the calculator will show you the expression that is used. You can copy this equation to a table in Post which will give you the same number. (Remove the additional spaces that come when copying from the function calculator.) This table can be part of the Report that can be saved for further processing outside Post.. An additional option is to add Text to a figure. In the text definition, you can add the expression as well. Then you have a figure with the volume as a number. 

November 14, 2021, 05:03 

#5  
New Member
Lukas
Join Date: Sep 2021
Posts: 9
Rep Power: 2 
Quote:
Is there a work around? I've been trying to get around it for several hours but couldn’t find a way yet. As always: thanks in advance, GertJan. 

November 14, 2021, 05:56 

#6 
Senior Member
GertJan
Join Date: Oct 2012
Location: Europe
Posts: 1,388
Rep Power: 21 
You can create an expression with stepfunctions with geometrical limits for clipping.
Say your isosurface is the air volume fraction 0.99 and only want to see it above z=1, above y=0 and above x=0. Then you can create an expression something like; airvfxyzlimit = Air.Volume Fraciton*step(z/1[m]1)*step(y/1[m])*step(x/1[m]) Then go to the tab Variables, create a new variable like AirVFxyzlimit and let it refer to your expression airvfxyzlimit Then go to your isosurface, and use the geometrically limited variable on the value 0.99. If your x, y and z limits have the right values, then you only see the small isosurface that you want. Now to determine the volume within this isosurface, use the geometrically limited variable in the expression. ___________ P.S. In principle, you don't need the new variable, since you can determine the volume right away from the geometrically limited expression. But a visual confirmation of what you are doing is correct, will help a lot in the beginning. 

November 14, 2021, 07:08 

#7  
New Member
Lukas
Join Date: Sep 2021
Posts: 9
Rep Power: 2 
Quote:
Its working like a charm! Thanks a lot, GertJan! 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
On the CFD market and trends  sbaffini  Main CFD Forum  16  September 1, 2020 11:16 
Using CFD Post for OpenFoam results  Karpfen  OpenFOAM PostProcessing  3  January 19, 2018 09:48 
Postprocessing star ccm+ results in Ansys CFD Post  sidharath  STARCCM+  4  April 10, 2017 12:49 
Post processing in CFD Post or Fluent.  Blobs  OpenFOAM PostProcessing  2  June 26, 2016 08:23 
CFD Online Celebrates 20 Years Online  jola  Site News & Announcements  22  January 31, 2015 01:30 