|
[Sponsors] |
February 18, 2012, 13:36 |
functionObject file format
|
#1 |
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30 |
I can't seem to find a way to save the output of the functionObject "cuttingPlane" into a binary file. The default seems to be ASCII, which wastes disk space. Does anyone know if it's possible to change the file format?
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. |
|
February 18, 2012, 16:47 |
|
#2 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Hi Anton,
Nope! According to the code at "OpenFOAM-2.1.x/src/sampling/sampledSurface/writers", it's all hard coded as ASCII only. There is a proxy system, but it only sends the surface points to the writer. The closest you can get is pack things via another functionObject: http://openfoamwiki.net/index.php/Ti...ect_systemCall - this way you even pick the format you want well, compression only Best regards, Bruno
__________________
|
|
February 20, 2012, 07:55 |
|
#3 |
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30 |
Thanks Bruno! It's funny it's hard-coded to ASCII, because the writer classes do support binary files (at least src/conversion/ensight does). So for now I just hard-coded binary instead of ASCII, and it works fine
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. |
|
February 20, 2012, 09:52 |
|
#4 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Hi Anton,
I think they hard-coded things this way, because the normal writers are for volumes only Best regards, Bruno
__________________
|
|
February 22, 2012, 15:19 |
|
#5 |
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30 |
Sorry, I didn't quite get that. Can you explain what you mean with volumes only and normal writers?
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. |
|
February 22, 2012, 16:48 |
|
#6 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Quote:
Here's an example of what I'm talking about: http://www.cfd-online.com/Forums/ope...tml#post343937 If you read the whole thread, you'll understand that the sampled surface cannot be represented as nicely as a patch surface, simply because said sampled surface is only represented by points! I think this is why the functionObject "cuttingPlane" is using dedicated and hard-coded surface writers, instead of using an already existing "driver".
__________________
|
||
February 24, 2012, 06:25 |
|
#7 |
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30 |
Actually, I just noticed that the sample 'sampleDict' changed between 2.0.x and 2.1.x. The latter now includes an entry
Code:
39 // optionally define extra controls for the output formats 40 formatOptions 41 { 42 ensight 43 { 44 format binary; 45 } 46 }
__________________
*On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer. Last edited by akidess; February 24, 2012 at 07:44. Reason: formatting |
|
February 24, 2012, 09:51 |
|
#8 |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Nice! I should have looked deeper into this
__________________
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
2.0.x on Mac OSX | niklas | OpenFOAM Installation | 74 | March 28, 2012 17:46 |
"parabolicVelocity" in OpenFoam 2.1.0 ? | sawyer86 | OpenFOAM Running, Solving & CFD | 21 | February 7, 2012 12:44 |
OpenFOAM 1.7.1 installation problem on OpenSUSE 11.3 | flakid | OpenFOAM Installation | 16 | December 28, 2010 09:48 |
Problem with rhoSimpleFoam | matteo_gautero | OpenFOAM Running, Solving & CFD | 0 | February 28, 2008 07:51 |
error while compiling the USER Sub routine | CFD user | CFX | 3 | November 25, 2002 16:16 |