CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Copying/tessellating solution data

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   February 21, 2017, 14:50
Default Copying/tessellating solution data
  #1
New Member
 
Matthew
Join Date: Feb 2017
Posts: 4
Rep Power: 9
msandli is on a distinguished road
All,

I have searched for quite a while for an answer to my question. I'm simulating a domain with very regular, repeated geometry. In order to speed up my grid independence studies, I've broken down my domain into a "unit cell" in order to use the least number of cells possible.

Now that I've found my grid density, I want to apply it to the entire domain and use the results of the mesh convergence as my initial condition. Copying the mesh itself is easy enough in ICEM. However, is there a way to copy my .dat files in a similar way?

I would think it would take some sort of journal file manipulation, but since I can't actually open a .dat file to see what it is, I don't know how to do it. Basically, I want to copy the fluid properties at each point in the domain and paste them a certain delta-x and delta-y.

The reason I'm doing this is because my simple "unit cell" used for the mesh convergence study has essentially symmetric BC's on all 4 sides, but my larger geometry would have actual wall BC's at it's extents.

Thanks
msandli is offline   Reply With Quote

Old   February 21, 2017, 21:50
Default
  #2
Senior Member
 
Lucky
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 5,654
Rep Power: 65
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
It's been years since I've done it so I don't remember the exact steps. You should try this to see if it works for a simple case before trying to write it in a journal.

You load the case and data in Fluent. Translate your mesh, which has the effect of translating all the data with it. Save this new translated case if needed.

Then you import the original case and append it to the current case. Then merge them (boundaries and zones). Rinse & repeat.
LuckyTran is offline   Reply With Quote

Old   February 22, 2017, 01:30
Default
  #3
New Member
 
Matthew
Join Date: Feb 2017
Posts: 4
Rep Power: 9
msandli is on a distinguished road
I think you've shown me the way, thank you!

If anyone else is watching this, here's what I found worked:

Do as tran says, translate your mesh the desired distance. Then append your case and data files. This will give you a bunch of matching zones with suffixes added on - wall & wall.1, fluid & fluid.1, etc.

In my case, I needed to merge those zones to ease pre- and post-processing. When merging zones via the GUI, it is best to work your way down the list - fluid zones, interior zones, wall zones, etc. This will eliminate "unable to merge" errors between things that are lower down on the list.

Then, just make sure you turn the inside boundaries into the needed type of interface zones. For me, that was matched interface zones (even though my mesh is mapped and identical on either side of the interface, I needed to specify this manually to actually get flow across this new boundary).

Thanks again!.
msandli is offline   Reply With Quote

Reply

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
Extracting data along polylines in transient solution blidblid CFX 1 July 27, 2016 03:05
2way FSi, Initialize with steady solution, Fluent, Transient Sturcural, System Coupli mmkkeshavarzi FLUENT 0 June 22, 2016 09:26
[OpenFOAM] Paraview doesn't seem to be picking up data generated by icofoam MikeHersee ParaView 2 January 6, 2015 09:27
Naca 0012 (compressible and inviscid) flow convergence problem bipulsaha FLUENT 1 July 6, 2011 08:51
PLOT3D ASCII solution file to MATLAB data file Sandeep Rana Main CFD Forum 4 June 11, 2010 10:48


All times are GMT -4. The time now is 11:01.