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

error in comments section of externalWallHeatFluxTemperature.H?

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

Like Tree1Likes
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 14, 2016, 14:26
Default error in comments section of externalWallHeatFluxTemperature.H?
  #1
Senior Member
 
Pei-Ying Hsieh
Join Date: Mar 2009
Posts: 322
Rep Power: 15
phsieh2005 is on a distinguished road
Hi,

The usage of externalWallHeatFluxTemperature is the following:
<patchName>
{
type externalWallHeatFluxTemperature;
kappa fluidThermo;
q uniform 1000;
Ta uniform 300.0;
h uniform 10.0;
thicknessLayers (0.1 0.2 0.3 0.4);
kappaLayers (1 2 3 4);
value uniform 300.0;
kappaName none;
Qr none;
relaxation 1;
}
\endverbatim

Note:
- Only supply \c h and \c Ta, or \c q in the dictionary (see above)
- \c kappa and \c kappaName are inherited from temperatureCoupledBase.
------------
But, I got an error of "kappaMethod is undefined. I need to change to
kappaMethod fluidThermo;

Is this a typo error?

Pei-Ying
phsieh2005 is offline   Reply With Quote

Old   August 18, 2016, 13:49
Default
  #2
Member
 
Pedro
Join Date: Nov 2014
Posts: 50
Rep Power: 8
pupo is on a distinguished road
Seems that the instructions are not updated, but the code is not consistant either. there is no "kappaMethod" here: https://github.com/OpenFOAM/OpenFOAM...hScalarField.C

the following sintax works for a fixed heat transfer heated wall:


Code:
   "fluid_to_.*"  
   { 
      type             externalWallHeatFluxTemperature;
      kappa            fluidThermo; 
      kappaMethod      fluidThermo;
      q                uniform 264; 
      value            uniform 293.7;
   }
pupo is offline   Reply With Quote

Old   August 20, 2016, 14:54
Default
  #3
Retired Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,962
Blog Entries: 45
Rep Power: 125
wyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to allwyldckat is a name known to all
Quick answer: Unfortunately that's one example of having the same documentation in several places. When one if fixed, all others may or may not be updated.

If you follow the link online for the "temperatureCoupledBase" class, you'll find the description here: http://cpp.openfoam.org/v4/a02649.html#details

The change that occurred was reported in the following commit: https://github.com/OpenFOAM/OpenFOAM...e92188c3953b8e
Quote:
temperatureCoupledBase: Rationalized the selection of the method for obtaining the thermal conductivity

Code:
kappa -> kappaMethod
kappaName -> kappa
I'll submit a patch for 4.x and dev in a few minutes and update this post accordingly.

Furthermore, next time you pick-up this kind of typo, please do report it at http://bugs.openfoam.org

edit: Patch has been submitted here: http://bugs.openfoam.org/view.php?id=2207
vs11 likes this.
__________________

Last edited by wyldckat; August 20, 2016 at 16:30. Reason: see "edit:"
wyldckat 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
[Commercial meshers] converting Fluent mesh to openfoam standard mesh deepesh OpenFOAM Meshing & Mesh Conversion 31 March 29, 2017 05:59
dsmcInitialise - dsmcFoam archymedes OpenFOAM Pre-Processing 94 July 15, 2016 16:14
[Other] How to create an MRF zone ? aminem OpenFOAM Meshing & Mesh Conversion 2 December 8, 2014 10:45
udf-Surface Reaction Rate-parse error in line 34 priya_1985 FLUENT 1 November 10, 2014 02:48
LiftDrag utility from v12 to v141 cfdphil OpenFOAM Running, Solving & CFD 2 December 5, 2007 05:49


All times are GMT -4. The time now is 06:17.