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

error in comments section of externalWallHeatFluxTemperature.H?

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

Reply
 
LinkBack Thread Tools 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: 313
Rep Power: 10
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: 46
Rep Power: 3
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
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,557
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
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
__________________

Last edited by wyldckat; August 20, 2016 at 16:30. Reason: see "edit:"
wyldckat is offline   Reply With Quote

Reply

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
dsmcInitialise - dsmcFoam archymedes OpenFOAM Pre-Processing 94 July 15, 2016 16:14
converting Fluent mesh to openfoam standard mesh deepesh OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 25 June 27, 2016 00:58
How to create an MRF zone ? aminem OpenFOAM Meshing & Mesh Conversion 2 December 8, 2014 11:45
udf-Surface Reaction Rate-parse error in line 34 priya_1985 FLUENT 1 November 10, 2014 03:48
LiftDrag utility from v12 to v141 cfdphil OpenFOAM Running, Solving & CFD 2 December 5, 2007 06:49


All times are GMT -4. The time now is 17:12.