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

Mesh area/volume calculations

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 14, 2016, 12:45
Default Mesh area/volume calculations
  #1
New Member
 
acalado's Avatar
 
André
Join Date: Mar 2016
Posts: 25
Rep Power: 2
acalado is on a distinguished road
Greetings,

I am quite new to StarCCM and I am working with flow in porous media.

One of the quantities of interest is the specific area (m2/m3) of the medium, and I was wondering if I could obtain this by dividing the total surface area of the mesh (which is already defined) by its occupied volume.

In theory this should not be quite accurate since it will not compute the solid volume, only the fluid, but still I would like to know if this is possible and easy to do just to get an idea.



Thanks in advance for any response!
__________________
Sapere aude!
acalado is offline   Reply With Quote

Old   March 15, 2016, 15:11
Default
  #2
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 563
Rep Power: 7
MBdonCFD is on a distinguished road
you should be able to setup reports and field functions to get this. Is it simply the face area / volume of the media?
MBdonCFD is offline   Reply With Quote

Old   March 15, 2016, 15:50
Default
  #3
New Member
 
acalado's Avatar
 
André
Join Date: Mar 2016
Posts: 25
Rep Power: 2
acalado is on a distinguished road
Quote:
Originally Posted by MBdonCFD View Post
you should be able to setup reports and field functions to get this. Is it simply the face area / volume of the media?
Thanks for the answer.

After some thought I'm thinking it should be not the total cell area, but only wall bounded surfaces (wall surface / total volume )

Possibly there should be some function to compute total wall area of a certain region...
__________________
Sapere aude!
acalado is offline   Reply With Quote

Old   March 15, 2016, 16:15
Default
  #4
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 563
Rep Power: 7
MBdonCFD is on a distinguished road
This should be fairly straight forward...

1. Create a new sum report, title it A.
2. Assign Area: Magnitude as your scalar field function.
3. Assign region boundaries that make up your surface area. Make sure to select the interfaces where the porous region/fluid regions meet as well as any frames or walls that bound the outside. (See attachment).
4. Right click report A, select Run... and make sure the value makes sense.
5. Next, create a new sum report and title it V.
6. Assign volume as your scalar field function.
7. Assign your entire porous region as the input part.
8. Again, run the report and make sure the value makes sense.
9. Finally, create a new expression report and rename it specificA.
10. Assign dimensions of L=-1.
11. Define the function as ${AReport}/${VReport}


You can then treat that report like any other... run it, create an annotation, etc...
Attached Images
File Type: png selections.png (159.7 KB, 12 views)
MBdonCFD is offline   Reply With Quote

Old   March 16, 2016, 09:39
Default
  #5
New Member
 
acalado's Avatar
 
André
Join Date: Mar 2016
Posts: 25
Rep Power: 2
acalado is on a distinguished road
Thanks very much!

Just one problem: The volume calculation should be pretty straight-forward, I'm using a cylinder as the boundary, so it's a simple calculation, however when I choose Parts -> Cylinder the computed volume is 0.

Any suggestions?
__________________
Sapere aude!
acalado is offline   Reply With Quote

Old   March 16, 2016, 09:47
Default
  #6
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 563
Rep Power: 7
MBdonCFD is on a distinguished road
are you selecting the part or the region? that can make a difference. make sure you select region boundaries and not part surfaces
MBdonCFD is offline   Reply With Quote

Old   March 16, 2016, 09:48
Default
  #7
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 563
Rep Power: 7
MBdonCFD is on a distinguished road
Sorry, not boundaries for volume. Just the region itself. Take a look at my attached image from earlier, it should illustrate the difference.
MBdonCFD is offline   Reply With Quote

Reply

Tags
foam, mesh, porous, specific area

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
[ICEM] surface mesh merging problem everest ANSYS Meshing & Geometry 44 April 14, 2016 06:41
decomposePar problem: Cell 0contains face labels out of range vaina74 OpenFOAM Pre-Processing 27 November 2, 2015 18:04
sliding mesh problem in CFX Saima CFX 45 September 22, 2015 10:53
[ICEM] Problem making structural mesh on a surface froztbear ANSYS Meshing & Geometry 1 November 10, 2011 09:52
snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Native Meshers: snappyHexMesh and Others 2 March 27, 2011 21:11


All times are GMT -4. The time now is 09:23.