CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

externalWallHeatFluxTemperature

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

Like Tree3Likes
  • 2 Post By wyldckat
  • 1 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   May 5, 2014, 04:17
Default externalWallHeatFluxTemperature
  #1
Member
 
Roman
Join Date: Sep 2013
Posts: 42
Rep Power: 5
Roman1 is on a distinguished road
Hello. The function externalWallHeatFluxTemperature works differently at OF2.2 and at OF2.3 but the source code looks equal. Where one can find differences?
Roman1 is offline   Reply With Quote

Old   May 5, 2014, 04:20
Default
  #2
Member
 
Andrew Somorjai
Join Date: May 2013
Posts: 77
Rep Power: 5
massive_turbulence is on a distinguished road
Quote:
Originally Posted by Roman1 View Post
Hello. The function externalWallHeatFluxTemperature works differently at OF2.2 and at OF2.3 but the source code looks equal. Where one can find differences?

What exactly do you mean "works differently"? Are the enumerators different in terms of words used to describe the object? Did you get different results using the same dictionary file?
massive_turbulence is offline   Reply With Quote

Old   May 5, 2014, 04:26
Default
  #3
Member
 
Roman
Join Date: Sep 2013
Posts: 42
Rep Power: 5
Roman1 is on a distinguished road
Yes, I get different results at Of2.2 and OF2.3 with the same case. The function wallHeatFlux shows greater values at OF2.3 and the temperature inside the domain at OF2.2 higher that at OF2.3.
Roman1 is offline   Reply With Quote

Old   May 5, 2014, 11:46
Default
  #4
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 266
Rep Power: 10
olivierG is on a distinguished road
hello,
Not sure here, but i think there were a bug report about this bc for OF2.2

regards,
olivier
olivierG is offline   Reply With Quote

Old   May 28, 2014, 05:57
Default
  #5
Member
 
Roman
Join Date: Sep 2013
Posts: 42
Rep Power: 5
Roman1 is on a distinguished road
The bug is in OF2.3: http://www.openfoam.org/mantisbt/view.php?id=1258
Thanks to all
Roman1 is offline   Reply With Quote

Old   May 31, 2014, 15:03
Default
  #6
Senior Member
 
Derek Mitchell
Join Date: Mar 2014
Location: UK, Reading
Posts: 139
Rep Power: 6
derekm is on a distinguished road
how does one get a fixed version of this in openfoam?
__________________
A CHEERING BAND OF FRIENDLY ELVES CARRY THE CONQUERING ADVENTURER OFF INTO THE SUNSET
derekm is offline   Reply With Quote

Old   June 2, 2014, 03:17
Default
  #7
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 266
Rep Power: 10
olivierG is on a distinguished road
Just use the 2.3.x version from git repo.
Then a git pull and Allwmake will give you a up to date version.

regards,
olivier
olivierG is offline   Reply With Quote

Old   June 2, 2014, 15:48
Default
  #8
New Member
 
Jean El-Hajal
Join Date: Jun 2010
Location: Ulm
Posts: 16
Rep Power: 8
Jean El-Hajal is on a distinguished road
Dear all,

are you using the externalWallHeatFluxTemperature function with the heat flux (q) option or with the heat transfer coefficient (h) and external temperature (Ta) option ?

With the heat flux (q) it seems to work. But with the heat transfer coefficient (h) and external temperature (Ta) it works with OpenFoam 2.2.2 but not with OpenFoam 2.3.0. With OF 2.3.0 it just behave like an adiabatic wall ?! Did someone test this option with OF 2.3.0 ?

Best regards,

Jean
Jean El-Hajal is offline   Reply With Quote

Old   June 3, 2014, 00:41
Default
  #9
Member
 
Roman
Join Date: Sep 2013
Posts: 42
Rep Power: 5
Roman1 is on a distinguished road
The bug is in OF2.3: http://www.openfoam.org/mantisbt/view.php?id=1258
Roman1 is offline   Reply With Quote

Old   November 20, 2014, 03:20
Default
  #10
Senior Member
 
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 713
Rep Power: 15
vasava will become famous soon enough
I have installed openFoam by following instructions on the openFoam website. I do not wish to go through the installation process again. Is there any workaround to use the corrected boundary condition??
vasava is offline   Reply With Quote

Old   March 27, 2015, 13:19
Default
  #11
Member
 
Naresh Yathuru
Join Date: Feb 2015
Posts: 63
Rep Power: 4
Naresh yathuru is on a distinguished road
Hi Foamers,

I m also using OF 2.3.0 and I have the same problem like vasava. could someone please help me how to clear the bug with out re installing again. I m afraid if i have to reinstall openFoam again. because i m using centOS 6.5 and i struggled a lot during the previous installation. and i m not a very good user of linux os.

regards,
Naresh
Naresh yathuru is offline   Reply With Quote

Old   March 30, 2015, 06:04
Default ExternalwallHeatfluxtemperature BC in openFoam 2.3.0
  #12
Member
 
Naresh Yathuru
Join Date: Feb 2015
Posts: 63
Rep Power: 4
Naresh yathuru is on a distinguished road
Hi Foamers,
sorry for restarting the thread again. I have a similar problem with externalwallheatFluxTemperature. Could somebody help me. I have a question in this link.

http://www.cfd-online.com/Forums/ope...tml#post538568

I m using OF 2.3.0. and I read in some threads that there is a bug in 2.3.0. could someone tell me if which of the following a better idea to fix the bug.

1. make new boundary condition by copying the bounday condition from 2.3.1 into 2.3.0?
2. reinstall from git repository? if this is better then how?

3. can i use the boundary condition for incompressible solver?(buoyantboussinessqsimplefoam)

I m feel lost now.

regards,
Naresh Yathuru

[Moderator note: post moved from the thread http://www.cfd-online.com/Forums/ope...bient-air.html ]

Last edited by wyldckat; April 5, 2015 at 07:48. Reason: see "Moderator note:"
Naresh yathuru is offline   Reply With Quote

Old   April 5, 2015, 08:15
Default
  #13
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,860
Blog Entries: 39
Rep Power: 108
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Hi Naresh,

Quote:
Originally Posted by Naresh yathuru View Post
1. make new boundary condition by copying the bounday condition from 2.3.1 into 2.3.0?
I don't know if you've already solved this problem or not, but the easiest is to follow these steps:
  1. Run these commands, for going to the folder for fixing the damaged boundary condition:
    Code:
    cd $FOAM_SRC/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/externalWallHeatFluxTemperature/
  2. Backup the current file:
    Code:
    mv externalWallHeatFluxTemperatureFvPatchScalarField.C externalWallHeatFluxTemperatureFvPatchScalarField.C.old
  3. Download the file that has the fixed file:
    Code:
    wget --no-check-certificate https://raw.githubusercontent.com/OpenFOAM/OpenFOAM-2.3.x/master/src/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/externalWallHeatFluxTemperature/externalWallHeatFluxTemperatureFvPatchScalarField.C
  4. Now build the library that needs to be fixed:
    Code:
    cd $FOAM_SRC/turbulenceModels/compressible/turbulenceModel
    wmake libso
  5. Run the last command again:
    Code:
    wmake libso
    it should tell you something like this:
    Code:
    '/home/ofuser/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so' is up to date.
    which means that it's fixed.
And it should now work correctly.


Best regards,
Bruno
flowAlways and Naresh yathuru like this.
__________________
wyldckat is offline   Reply With Quote

Old   April 7, 2015, 08:05
Default
  #14
Member
 
Naresh Yathuru
Join Date: Feb 2015
Posts: 63
Rep Power: 4
Naresh yathuru is on a distinguished road
hello Bruno,

thank you for the reply once again. I was interested in using the externalwallHeatFluxTemperature for incompressible flows. but as far as i have read it works only for compressible solver and in addition to that there is a bug. so i was trying something with grooveyBC but without sucess.

Now i should get back to square 1, and try to implement the b.c for incompressible solvers. I know its really hard for someone like me who doesnt have a very good knowledge of c++.However i will try it sooner or later. i have started making changes to some basic solvers. i m comparing compressible ::turbulent'WallHeatTemperature B.C with incompressible:: turbulentWallHeatfluxTemperature B.C.


May be this is not an appropriate thread to ask this question. sorry but,It would be very helpful if someone had already implemented could post the B.c or any guidence on how to implenent it.

thanks once again Bruno and other Foamers.

Best Regards,
Naresh
Naresh yathuru is offline   Reply With Quote

Old   May 22, 2015, 11:55
Default
  #15
New Member
 
Ali Kadar
Join Date: Oct 2014
Location: Delft
Posts: 25
Rep Power: 4
flowAlways is on a distinguished road
Thanks Bruno,

Your solution works when we make changes to the FOAM_SRC, however since its not a good idea to make changes to the actual source. I copy the directory $FOAM_SRC/turbulenceModels/compressible/turbulenceModel make changes to externalWallHeatFluxTemperatureFvPatchScalarField. C and update
LIB = $(FOAM_USER_LIBBIN)/libmy_compressibleTurbulenceModel in Make/files.

However the build with "wmake libso" exits with the following error
Code:
derivedFvPatchFields/externalWallHeatFluxTemperature/externalWallHeatFluxTemperatureFvPatchScalarField.C:72:  error: class ‘Foam::externalWallHeatFluxTemperatureFvPatchScalarField’  does not have any field named ‘QrName_’
I think Qr for radiation was implemented in version 2.3.1 and is not present in 2.3.0 ... and therefore the make fails... can you please suggest a way, what more changes would be needed for a successful build ?








Quote:
Originally Posted by wyldckat View Post
Hi Naresh,


I don't know if you've already solved this problem or not, but the easiest is to follow these steps:
  1. Run these commands, for going to the folder for fixing the damaged boundary condition:
    Code:
    cd $FOAM_SRC/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/externalWallHeatFluxTemperature/
  2. Backup the current file:
    Code:
    mv externalWallHeatFluxTemperatureFvPatchScalarField.C externalWallHeatFluxTemperatureFvPatchScalarField.C.old
  3. Download the file that has the fixed file:
    Code:
    wget --no-check-certificate https://raw.githubusercontent.com/OpenFOAM/OpenFOAM-2.3.x/master/src/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/externalWallHeatFluxTemperature/externalWallHeatFluxTemperatureFvPatchScalarField.C
  4. Now build the library that needs to be fixed:
    Code:
    cd $FOAM_SRC/turbulenceModels/compressible/turbulenceModel
    wmake libso
  5. Run the last command again:
    Code:
    wmake libso
    it should tell you something like this:
    Code:
    '/home/ofuser/OpenFOAM/OpenFOAM-2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so' is up to date.
    which means that it's fixed.
And it should now work correctly.


Best regards,
Bruno
__________________
A good solution is one which does justice to the inner nature of the problem- Cornelius Lanczos in a letter to Albert Einstein on March 9, 1947
flowAlways is offline   Reply With Quote

Old   May 24, 2015, 09:27
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,860
Blog Entries: 39
Rep Power: 108
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Greetings flowAlways,

Sorry, but I'll have to be quick: you're doing the right thing in not modifying the original source code directly, but you should not copy the source code for the whole library, otherwise you risk in-process memory corruption, due to having objects with the same name.

You should instead to it as explained here: http://openfoamwiki.net/index.php/Ho...dary_condition
which is to make a copy of only the relevant files you need to fix.

In addition, I guess that the fix I proposed in the previous post only repairs the ".C" file. Therefore, you should also update the ".H" file.

Best regards,
Bruno
flowAlways likes this.
__________________
wyldckat is offline   Reply With Quote

Old   July 28, 2015, 09:57
Default It works
  #17
New Member
 
Matthias Hettel
Join Date: Apr 2011
Location: Karlsruhe, Germany
Posts: 28
Rep Power: 8
matthi is on a distinguished road
Hi Foamers,

if you also update externalWallHeatFluxTemperatureFvPatchScalarField. H it works.

Greetings matthi
matthi is offline   Reply With Quote

Old   April 3, 2017, 06:11
Default
  #18
New Member
 
Akshay
Join Date: Nov 2016
Location: Chennai,India
Posts: 7
Rep Power: 2
vak96 is on a distinguished road
Hi Foamers,

I want to use externalWallHeatFluxTemperature boundary condition for my own customized laplacian solver. Can anyone please explain in detail, how to apply that boundary condition? I know that it has been used in few tutorial problem but I could not get exactly how to use it.

I am using Openfoam-v1612+ and my geometry is a cylinder. I want this boundary condition for walls.

I will be very happy if someone helps me.

Thanking you in advance,
Akshay
vak96 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



All times are GMT -4. The time now is 21:23.