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

external wall heat transfer

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

Like Tree1Likes
  • 1 Post By olivierG

Reply
 
LinkBack Thread Tools Display Modes
Old   January 23, 2014, 04:17
Default external wall heat transfer
  #1
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Hello,

I am actually trying to implement a boundary condition with heat transfer through the external wall. The equation is

Code:


Tw=(Tair-(alphain+(l/d)+alphaout)(Tair-Tinf))/alphain
 
 where Tw = wall temperature
 
 Tair = air temperature (calculated from the solver)
 alphain = heat transfer coefficient on the inside of the wall( calculated from the solver)
 l= thermal conductivity;
 d= virtual wall thickness;
 alphaout=heat transfer coefficient on the outside of the wall
 Tinf= outside temperatue


Has anybody got any idea on how to implement this BC using groovy? with alphain and Tair generating from the solver. Till now I have tried something like this:


Code:


wand2
    {
        type groovyBC;
        value uniform 293.15;
       fractionExpression "0";
       variables "alphaa=20;Tinf=300;d=0.015;l=23;Tw=(Tair-(alphain+(l/d)+alphaout)(Tair-Tinf))/alphain";
                    timelines (
                    );
}


which does'nt work and gives me an error like this


Code:
--> FOAM FATAL ERROR: 
 Parser Error for driver PatchValueExpressionDriver at "1.30" :"syntax error, unexpected '('"
"(Tair-(alphaa+(l/d)+alphaout)(Tair-Tinf))/alphaa"
                               ^
-------------------------------|

Context of the error:


- From dictionary: /home/ashwin/Desktop/wallbc/0/T.boundaryField.wand2
  Evaluating expression "(Tair-(alphaa+(l/d)+alphaout)(Tair-Tinf))/alphaa"


    From function parsingValue
    in file lnInclude/CommonValueExpressionDriverI.H at line 1081.

FOAM exiting




I am using buoyantSimpleFoam Solver. I have no idea on how to generate the Tair and heat transfer coefficient from the solver.

I hope somebody here has an idea about it.


Regards
Ashwin


Last edited by ashghan; January 24, 2014 at 06:07. Reason: checked on how to post a thread :)
ashghan is offline   Reply With Quote

Old   January 29, 2014, 07:52
Default
  #2
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,076
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Ashwin,

hmmm your problem seems "easy".

First - the solver calculates Alpha (in the air Domain) and you will get the temperature of the wall.

You want to extend the wall with an thickness of "l" to simulate a pipe or sth like that and the heat Transfer from the pipe to the outer fluid (i think air).

So you will do a fluid - solid - fluid Simulation.

a) you can do it with chtMultiRegion
b) you can build your own BC - as you tried

In your case (b) you made some mistakes.

1. you do not calculate the heat Transfer from fluid to solid surface - that do the solver. Therefor you do not Need alphain.

2. Tair is not a OpenFOAM variable. I think you have to use "T" or "T()" instead.

3. I did not get your Point with Tw, Tair, Tinf. What do you want to achive? In my opinion you Need:

- conductivity
- Tinf
- Thickness


Any questions?
Regards Tobi
Tobi is offline   Reply With Quote

Old   January 29, 2014, 08:04
Default
  #3
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Hello Tobias,

First of All, Thank you for the reply.

Yeah I need conductivity, Thickness, The outside wall temperature = Tinf and the heat transfer coefficient on the outside = alphaout as a user input to calculate the Tw= wall temperature on the inside.

I am applying this to a Normal wall(with a thickness d) in a room, to calculate the inside wall temperature.


Regards
Ashwin
ashghan is offline   Reply With Quote

Old   January 29, 2014, 08:29
Default
  #4
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
I think you're trying to apply a mixedBC / Robin boundary condition: Mixed BC - heat transfer - laplacianFoam
__________________
*On twitter @akidTwit
*Spend as much time formulating your questions as you expect people to spend on their answer.
*Help define the OpenFOAM stackexchange Q&A site: http://area51.stackexchange.com/prop...oam-technology
akidess is offline   Reply With Quote

Old   January 29, 2014, 10:45
Default
  #5
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Quote:
Originally Posted by akidess View Post
I think you're trying to apply a mixedBC / Robin boundary condition: Mixed BC - heat transfer - laplacianFoam
Hello,

I am trying to do something similar to the external wall heat flux.

Regards
Ashwin
ashghan is offline   Reply With Quote

Old   January 29, 2014, 16:09
Default
  #6
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,076
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Ashwin,

hm ... hmmm i am a bit confused

Just to clear my mind. You want to bring heat energy into your system ?
Well alphaout you have to define yourself
Tobi is offline   Reply With Quote

Old   January 29, 2014, 17:23
Default
  #7
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Hello Tobias,

Yes I am bringing the heat Energy from outside the system and yeah I give alphaout, conductivity, thickness and outside temperature as a user input.

The alphain and Tair are derived from the solver. So when I use a Value expression like

Code:
Tw=(T-(alpha+(l/d)+alphaout)(T-Tinf))/alpha
It does'nt work. So how do I calculate the Tw?

http://www.flickr.com/photos/115947529@N08/12211738076/
ashghan is offline   Reply With Quote

Old   January 29, 2014, 18:03
Default
  #8
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,076
Blog Entries: 4
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by ashghan View Post
Hello Tobias,

Yes I am bringing the heat Energy from outside the system and yeah I give alphaout, conductivity, thickness and outside temperature as a user input.

The alphain and Tair are derived from the solver. So when I use a Value expression like

Code:
Tw=(T-(alpha+(l/d)+alphaout)(T-Tinf))/alpha
It does'nt work. So how do I calculate the Tw?

http://www.flickr.com/photos/115947529@N08/12211738076/

Hi you have a logical mistake.
You do not need Tw ... Tw is calculated from the solver!

Regards
Tobi
Tobi is offline   Reply With Quote

Old   January 30, 2014, 04:43
Default
  #9
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Quote:
Originally Posted by Tobi View Post
Hi you have a logical mistake.
You do not need Tw ... Tw is calculated from the solver!

Regards
Tobi
Hi,

Now I am using this piece of code

Code:
wand2
    
        {
                 type groovyBC;
                 value uniform 293.15;
                 variables "alphaout=20;Tinf=300;d=0.05;l=0.05;";
                 Value Expression "(T-(alpha+(l/d)+alphaout)*(T-Tinf))/alpha";
                 timelines       ();
               
                 }
and I get the following error

Code:
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::incompressiblePerfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:?
#4  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::incompressiblePerfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:?
#5  
 at ??:?
#6  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7  
 at ??:?
Floating point exception (core dumped)
Any ideas on this?

Regards
Ashwin
ashghan is offline   Reply With Quote

Old   January 30, 2014, 05:45
Default
  #10
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 235
Rep Power: 9
olivierG is on a distinguished road
hello,

Why you don't use the "externalWallHeatFluxTemperature" BC ?

regards,
olivier
olivierG is offline   Reply With Quote

Old   January 30, 2014, 05:49
Default
  #11
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Quote:
Originally Posted by olivierG View Post
hello,

Why you don't use the "externalWallHeatFluxTemperature" BC ?

regards,
olivier
Hello,

I tried to use that, but I am not getting good heat balance. The HeatFlux's seem to be bad.

Regards
Ashwin
ashghan is offline   Reply With Quote

Old   January 30, 2014, 06:18
Default
  #12
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 235
Rep Power: 9
olivierG is on a distinguished road
hello,

If something is wrong with "externealWallHeatFluxTemperature", you may report as a bug. This will help all OF user, including you.

If you use use groovyBC, you may follow the advice from Akidess:
Code:
type groovyBC;
value uniform 293.15;
variables "alphaout=20;Tinf=300;d=0.05;l=0.05;alphawall=l/d;K=DT*rho*Cp;htot=alphaout+alphawall;";
valueExpression "Tinf";
fractionExpression "1.0/(1.0 + K/(mag(delta())*htot))";
NB: you need to adapt the conductivity "DT" name, density "rho" and "Cp" name.

regards,
olivier
olivierG is offline   Reply With Quote

Old   January 30, 2014, 06:34
Default
  #13
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Hello Oliver,

I have a question from your code.

Why do we need DT and K ? Since l is the thermal conductivity provided.

Regards
Ashwin
ashghan is offline   Reply With Quote

Old   January 30, 2014, 06:45
Default
  #14
Senior Member
 
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 235
Rep Power: 9
olivierG is on a distinguished road
Hello,

Check and read the link from Akidess for more info.
DT, rho , Cp are for the bulk properties.

regards,
olivier
akidess likes this.
olivierG is offline   Reply With Quote

Old   January 30, 2014, 11:11
Default
  #15
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Hello Tobias, Akidess and Oliver,

I have another question regarding external wall heat flux temperature. Can I input Q in [W/m] instead of [W/m] making it as a volumetric source term?

Regards
Ashwin
ashghan is offline   Reply With Quote

Old   January 31, 2014, 10:17
Default
  #16
New Member
 
ashwin
Join Date: Jul 2012
Location: erlangen
Posts: 25
Rep Power: 4
ashghan is on a distinguished road
Hello,

My Expression is working when I use h instead of alpha. Is it correct? I took it as h w.r.t to convective heat transfer coefficient notation. Please leme know if I am wrong.

Code:
valueExpression "(T-(h+(l/d)+alphaout)*(T-Tinf))/h";
If I use alpha I get an error saying

Code:
Parser Error for driver PatchValueExpressionDriver at "1.5-9" :"field alpha not existing or of wrong type"
Regards
Ashwin
ashghan 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
Two-sided Wall Heat Transfer BC - No Separate Solid Mesh and No Heat Transfer Coeff swahono OpenFOAM Running, Solving & CFD 8 February 26, 2015 05:30
Radiation interface hinca CFX 15 January 26, 2014 18:11
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
Convective / Conductive Heat Transfer in Hypersonic flows enigma Main CFD Forum 2 November 1, 2009 23:53
WALL HEAT TRANSFER COEF...AGAIN Carl CFX 2 July 8, 2005 01:35


All times are GMT -4. The time now is 03:17.