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

How to get wall heat flux from reactingFoam?

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

Like Tree6Likes
  • 2 Post By dlahaye
  • 3 Post By Yann
  • 1 Post By dlahaye

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 24, 2022, 05:58
Question How to get wall heat flux from reactingFoam?
  #1
New Member
 
mactone hsieh
Join Date: Apr 2012
Location: Taiwan
Posts: 18
Rep Power: 12
mactone is on a distinguished road
Dear OpenFomers,

I build a fluid domain for combustion simulation using reactingFoam.
When I tried to use
Code:
postProcess -func wallHeatFlux
I can't get the heat flux from the wall.

Code:
--> FOAM FATAL ERROR: (openfoam-2206)
Unable to find compressible turbulence model in the database

   From virtual bool Foam::functionObjects::wallHeatFlux::execute()
   in file wallHeatFlux/wallHeatFlux.C at line 255.

FOAM exiting
Is it the reactingFoam issue? or my boundary condition issue?

By the way, I've tested the wall boundary set at contant temperature or externalWallHeatFluxTemperature. Both boundary can't postProcess wallHeatFlux.

Thank you formers!
mactone is offline   Reply With Quote

Old   August 24, 2022, 08:44
Default
  #2
Senior Member
 
Domenico Lahaye
Join Date: Dec 2013
Posts: 517
Blog Entries: 1
Rep Power: 14
dlahaye is on a distinguished road
1/ Suggestion 1

Place wallHeatFlux computation in system/controlDict as in

Code:
<existing controlDict>
functions
{
    #includeFunc wallHeatFlux 
}
Motivation: this approach uses a default wallHeatFlux file (details missing) that provide the path to the correct shared object library.

2/ Suggestion 2

Add to Suggestion 1 your own wallHeatFlux file (thus overriding the default). Example is in the squareBend tutorial of rhoSimpleFoam. Observe that libs is set to fieldFunctionObjects.

3/ Suggestion 3 (requiring more witchcraft)

Verify that the wallHeatFlux function is indeed provided by the shared object file as the wallHeatFlux tells us.

fieldFunctionObjects is in the directory openfoam2012/platforms/linux64GccDPInt32Opt/lib .

To verify that wallHeatFlux is indeed provided, use

nm -g libfieldFunctionObjects.so | grep -I wallheatflux

Let us know what you learn.
Yann and mactone like this.
dlahaye is offline   Reply With Quote

Old   August 24, 2022, 10:04
Default
  #3
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 578
Rep Power: 19
Yann will become famous soon enough
Hi,

In addition to Domenico's points, try running:

Code:
reactingFoam -postProcess -func wallHeatFlux
the postProcess utility loads the mesh and variables, but not the models related to your case. This is why it fails to execute functions objects which need to access model-related data.

In your case, postProcess utility does not load the turbulence model, but the wallHeatFlux function object needs it. When using reactingFoam -postProcess, the solver starts, loads all the models it needs, and then execute the function called by the -postProcess option.

I don't have experience with reactingFoam so other problems might arise, but this is worth trying.

Cheers,
Yann
jherb, mactone and dlahaye like this.
Yann is offline   Reply With Quote

Old   August 24, 2022, 21:33
Default
  #4
New Member
 
mactone hsieh
Join Date: Apr 2012
Location: Taiwan
Posts: 18
Rep Power: 12
mactone is on a distinguished road
Thank you @dlahaye and @Yann for such thorough procedures to solve my question.

I've tried using Yann's recommendation. It works. It will output a wallHeatFlux_step.dat in the postProcessing/wallHeatFlux folder.

The suggestion1 of dlahaye is also working. The wall heat flux will be output to another file wallHeatFlux.dat in the same directory with the same output frequency as the result file.

In the file, there are columns of time, patch, min, max, integral, it looks like below.

Code:
# Wall heat-flux  
# Time            	patch             	min               	max               	integral          
73605             	air	-1.0249754810e-01	2.2350346338e+00	4.4728118225e-02
73605             	fuel	-2.1019176497e+01	6.6393800060e+01	5.3537524375e-02
73605             	outlet1	0.0000000000e+00	0.0000000000e+00	0.0000000000e+00
73605             	outlet2	0.0000000000e+00	0.0000000000e+00	0.0000000000e+00
73605             	wall_burner	-9.8068755227e+04	6.0199488781e+02	-3.4648932558e+00
73605             	wall_chamber	-1.2467911377e+06	2.4665724705e+04	-3.0640880412e+05
The first 4 columns are descriptive. But I am not sure about the last column.
Does the 'integral' means the total heat flux through the path in unit of kW?
For the minus sign (-), it mean the heat is going out through the patch.
It makes me wonder, why there is plus (+) heat flux through wall_chamber (see the max)?


One other thing which might not related to the postProcessing.
I've asked reactingFoam with boundary heat transfer?
to know if the OpenFOAM can have thin wall heat transfer as that in fluent. If any former can share, it will be appreciated.
mactone is offline   Reply With Quote

Old   August 25, 2022, 03:57
Default
  #5
Senior Member
 
Domenico Lahaye
Join Date: Dec 2013
Posts: 517
Blog Entries: 1
Rep Power: 14
dlahaye is on a distinguished road
Yes on integral.

Yes on sign.

No idea on wall_chamber patch. Requires seeing details.

See other post for other question.
Yann likes this.
dlahaye is offline   Reply With Quote

Reply

Tags
combustion, reactingfoam, wall heat transfer

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
Best (easiest) way to implement a specific heat flux from a Wall to a Fluid region FoamerLuc OpenFOAM 3 February 24, 2021 06:07
Heat Flux versus Wall Heat Flux: inlet - outlet energy, different values jmenendez CFX 1 February 14, 2021 17:55
Which macro should I use to define the heat flux of a wall ? DEFINE_HEAT_FLUX or DEF hitzhwan Fluent UDF and Scheme Programming 2 December 25, 2020 10:27
Radiation interface hinca CFX 15 January 26, 2014 18:11
An error has occurred in cfx5solve: volo87 CFX 5 June 14, 2013 18:44


All times are GMT -4. The time now is 18:55.