CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Visualization & Post-Processing Software > EnSight

Overset mesh post-processing

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

Like Tree3Likes
  • 1 Post By kevincolburn
  • 2 Post By HHOS

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 19, 2017, 12:03
Question Overset mesh post-processing
  #1
Member
 
Join Date: Jul 2013
Posts: 67
Rep Power: 9
HHOS is on a distinguished road
Hello everybody!

I just want to ask if there is any way to do the postprocessing of fluent cases where the overset function is used. Until now, the little postprocessing I managed to do was inside Fluent. In Ensight, the full meshes are displayed, not just the used part, so to speak.

Do you know if they are developing something related to the topic?

Regards.
HHOS is offline   Reply With Quote

Old   May 20, 2017, 00:13
Default
  #2
Senior Member
 
kevincolburn's Avatar
 
Kevin Colburn
Join Date: Mar 2009
Location: The Woodlands, TX
Posts: 131
Rep Power: 13
kevincolburn is on a distinguished road
Most overset mesh methods utilize/store/maintain the complete mesh domain, but also generate a "BLANKING" flag or variable to denote elements which are completely or partially removed from the computational domain. So, typically, most overset solvers will export the complete domain to the mesh/grid file, but then create a blanking variable (commonly referred to iblanking) which allows post processing programs to turn off/hide/blank elements appropriately.

So, have a look at the variables from the solver, and there should typically be some type of blanking variable. Make sure that you export/read that variable into the post processing software, and utilize it to blank out the elements appropriately.

-kevin
HHOS likes this.
__________________
Kevin Colburn
Computational Engineering International, Inc.
www.ceisoftware.com
kevin@ensight.com
kevincolburn is offline   Reply With Quote

Old   May 23, 2017, 10:28
Default
  #3
Member
 
Join Date: Jul 2013
Posts: 67
Rep Power: 9
HHOS is on a distinguished road
Thank you very much for the tip. It actually worked very well.

In case it is useful for somebody:

Working with Fluent, I had to export the "Overset_cell_type" variable. With that variable I do a isovolume for values [1,2]; that way I get the domain cells that are identified as "Donor" and "Solve".

That isovolume part(s) are my usual domain parts to work with.
kevincolburn and wc34071209 like this.
HHOS is offline   Reply With Quote

Old   November 17, 2017, 03:29
Default
  #4
New Member
 
Ashish Maikhuri
Join Date: Nov 2017
Location: Dehradun
Posts: 1
Rep Power: 0
ashishgehu is on a distinguished road
can u please elaborate the procedure for ansys fluent . i want to export the data of fluent overset mesh solver to cfd post . please help me
ashishgehu is offline   Reply With Quote

Old   December 8, 2017, 02:15
Default Overset postprocessing
  #5
New Member
 
Chen Hao
Join Date: May 2017
Posts: 3
Rep Power: 5
Lenny is on a distinguished road
Hi, HHOS

Can you tell me what is your meaning of "isovolume value"? And I export the "overset_cell_type" values and I found that those value are not consistent with what they should be in the tutorial like 0,1,2,-1,-2. My value is always above zero and some of them are not even integer,something like 0.33,0.25,1.53,2.53. Did you meet this kind of problems? By the way, the FLUENT version I use is 18.1.
Lenny is offline   Reply With Quote

Old   December 8, 2017, 08:03
Default
  #6
Member
 
Join Date: Jul 2013
Posts: 67
Rep Power: 9
HHOS is on a distinguished road
Well, first, I have no clue about CFD-Post, but I guess the procedure must be similar to that used in CEI Ensight (or maybe ANSYS Ensight now?).

Lenny, the isovolume part is something to be done in Ensight. I find weird that the "overset cell type" has those values you are saying. Maybe you exported something else?

Regards
HHOS is offline   Reply With Quote

Old   December 8, 2017, 08:35
Default
  #7
New Member
 
Chen Hao
Join Date: May 2017
Posts: 3
Rep Power: 5
Lenny is on a distinguished road
Quote:
Originally Posted by HHOS View Post
Well, first, I have no clue about CFD-Post, but I guess the procedure must be similar to that used in CEI Ensight (or maybe ANSYS Ensight now?).

Lenny, the isovolume part is something to be done in Ensight. I find weird that the "overset cell type" has those values you are saying. Maybe you exported something else?

Regards
Thank you for your reply.
I checked my case again and I found that a information always come out when FLUENT exports data files. The information is:
"Overset connectivity information is only written to case files in HDF format. It is recommended that you write overset cases in HDF format(parallel solver required)". I don't know if that is the reason why those overset_cell_type values are not consistent with toturial. I will try to write date files into HDF format to see if it will work. Thank you.
Lenny is offline   Reply With Quote

Old   December 10, 2017, 21:28
Default Overset postprocessing
  #8
New Member
 
Chen Hao
Join Date: May 2017
Posts: 3
Rep Power: 5
Lenny is on a distinguished road
Hi,all! I get one problem solved. I figure out why overset_cell_type variables are not integer. That is because when I export data files into ASCII format, there is a "location" option(Node or Cell center) to specify the data location. I should have chosen Cell center instead of Node.
Lenny is offline   Reply With Quote

Reply

Tags
ensight, overset

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
Is overset mesh required? ahildershavn@yahoo.no OpenFOAM Running, Solving & CFD 2 August 4, 2017 03:23
Help in setting up an overset mesh RKE STAR-CCM+ 1 February 21, 2014 21:35
[snappyHexMesh] snappyHexMesh won't work - zeros everywhere! sc298 OpenFOAM Meshing & Mesh Conversion 2 March 27, 2011 21:11
Convergence moving mesh lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 14:09
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 14:19.