|
[Sponsors] |
May 22, 2013, 12:17 |
heat loss through wall : how to?
|
#1 |
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Dear OFoamers,
I'm trying to simulate a premixed mathane combustion in a cylindrical burner with XiFoam with OF 2.1.1. My chamber is a cylindre and I suppose the flow to be axisymmetric so I sat the geometry as a 2-D case with only a wedge of a cylindre. Now I'd like to take into account the heat loss through the wall. Could you please tell me what is the best way to do that? I hesitate between : 1. wallHeatTransfer Tinf 293 K alphaWall = 26 W/mK (it is sainless steel) value uniform 293 K 2. set a fixedGradient gradient uniform dTdr where dT/dr = Q/(A*k) with Q the heat flux, A the surface of the exchange between gas and water and k = alphaWall, the thermal conductivity . 3. other any better suggestion? Thank in advance Cam |
|
May 22, 2013, 12:31 |
|
#2 |
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 99
Rep Power: 14 |
I would prefer wallHeatTransfer over fixedGradient. I also had to choose between the two. If I remember correctly while monitoring the heat flux over the boundary the wallHeatFlux was correct from the beginning but for the fixedGradient it took some time/iterations for the boundary condition to be obeyed. In my case this was externalWallHeatFlux vs. fixedGradient.
|
|
May 22, 2013, 13:25 |
|
#3 |
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Well thank you for your response . I'll try this. Could you tell me what's the difference between wallHeatTransfer and externalWallHeatTransfer?
which one do I have to use in my case? it's to take into account the non adiabaticity of the burner. Are the next values correct? Tinf uniform 293; alphaWall uniform 26; value uniform 293 ; I don't understand what is the difference between Tinf and value? (whereas both seems to be required) |
|
May 22, 2013, 13:54 |
|
#4 | ||
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
I've just tried this and it does not seems to works I have many errors.. Maybe my other boundaries conditions aren't well defined?
first I have error such that the T is out of bound for the use of the JANAF coefficient : Quote:
Then I have mane other errors : Quote:
My BC are the next ones : for pressure : zeroGradient everywhere but at the internalField 1e5 for velocity U : - inlet : turbulentInlet 3 m/s - outlet :inletOutlet 0 0 0 - walls : fixedValue 0 0 0 for temperaure T : - inlet : fixedValue uniform 293 - outlet : type inletOutlet; inletValue uniform 293; value uniform 293; - walls : wallHeatTransfer as describe previously Well I would be grateful if someone could help me with that issue.. Thanks Cam |
|||
May 22, 2013, 14:15 |
|
#5 | |
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 99
Rep Power: 14 |
Quote:
For wallHeatTransfer you need to specify Tinf which is the wall temperature and alphaWall which is the thermal diffusivity. I think value is the initial temperature at the wall. So your alphaWall is probably wrong as the thermal diffusivity is defined as thermal conductivity / density / heat capacity [1] http://foam.sourceforge.net/docs/cpp/a02489.html |
||
May 22, 2013, 15:31 |
|
#6 | ||
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
ah ok and I m telling it the conductivity and not diffusivity
so for stainless steel I should put 4e-6 ?? (http://en.wikipedia.org/wiki/Thermal_diffusivity) Quote:
Quote:
Thank you for your advices. But I have some trouble to understand the source code :-/ |
|||
May 22, 2013, 16:06 |
|
#7 | ||
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 99
Rep Power: 14 |
Quote:
Quote:
If this is the initial temperature then yes. Sometimes there is a detailed description [1] on how to apply the boundary condition, if not you have to look it up in the source. [1] http://foam.sourceforge.net/docs/cpp...9.html#details |
|||
May 23, 2013, 03:10 |
|
#8 | |
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Dear Billie (or Daniel, as you prefer?)
Thank you again for your response. I don't see any value required in the documentation as OpenFoam 2.1.1 asks me on my computer. Quote:
Code:
#include "wallHeatTransferFvPatchScalarField.H" #include "addToRunTimeSelectionTable.H" #include "fvPatchFieldMapper.H" #include "volFields.H" #include "basicThermo.H" // * * * * * * * * * * * * * * * * Constructors * * * * * * * * * * * * * * // Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const fvPatch& p, const DimensionedField<scalar, volMesh>& iF ) : mixedFvPatchScalarField(p, iF), Tinf_(p.size(), 0.0), alphaWall_(p.size(), 0.0) { refValue() = 0.0; refGrad() = 0.0; valueFraction() = 0.0; } Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const wallHeatTransferFvPatchScalarField& ptf, const fvPatch& p, const DimensionedField<scalar, volMesh>& iF, const fvPatchFieldMapper& mapper ) : mixedFvPatchScalarField(ptf, p, iF, mapper), Tinf_(ptf.Tinf_, mapper), alphaWall_(ptf.alphaWall_, mapper) {} Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const fvPatch& p, const DimensionedField<scalar, volMesh>& iF, const dictionary& dict ) : mixedFvPatchScalarField(p, iF), Tinf_("Tinf", dict, p.size()), alphaWall_("alphaWall", dict, p.size()) { refValue() = Tinf_; refGrad() = 0.0; valueFraction() = 0.0; if (dict.found("value")) { fvPatchField<scalar>::operator= ( scalarField("value", dict, p.size()) ); } else { evaluate(); } } how can I know in which part of the code it is running? ie : Code:
Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const fvPatch& p, const DimensionedField<scalar, volMesh>& iF ) Code:
Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const wallHeatTransferFvPatchScalarField& ptf, const fvPatch& p, const DimensionedField<scalar, volMesh>& iF, const fvPatchFieldMapper& mapper ) Code:
Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const fvPatch& p, const DimensionedField<scalar, volMesh>& iF, const dictionary& dict ) Code:
Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const wallHeatTransferFvPatchScalarField& tppsf ) Code:
Foam::wallHeatTransferFvPatchScalarField::wallHeatTransferFvPatchScalarField ( const wallHeatTransferFvPatchScalarField& tppsf, const DimensionedField<scalar, volMesh>& iF ) |
||
May 23, 2013, 04:39 |
|
#9 | |||
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 99
Rep Power: 14 |
I don't mind
Quote:
Quote:
Quote:
|
||||
May 30, 2013, 04:25 |
|
#10 |
Member
Camille
Join Date: Oct 2012
Posts: 54
Rep Power: 13 |
Dear Daniel and other OpenFoamers,
I m asking myself another question about the wallHeatTransfer boundary condition. The burner I try to modelise is surrounded by an exchanger with water. since the heat transmitted to the wall and then to the water comes from the burnt specied (exhaust gas) shouldnt' I use the alpha of the species and not of the wall ? Cam |
|
June 4, 2013, 04:51 |
|
#11 | |
Member
Daniel Pielmeier
Join Date: Apr 2012
Posts: 99
Rep Power: 14 |
Quote:
[1] http://www.tufts.edu/as/tampl/en43/lecture_notes/ch4.html |
||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Radiation interface | hinca | CFX | 15 | January 26, 2014 17:11 |
Error finding variable "THERMX" | sunilpatil | CFX | 8 | April 26, 2013 07:00 |
[ICEM] Export ICEM mesh to Gambit / Fluent | romekr | ANSYS Meshing & Geometry | 1 | November 26, 2011 12:11 |
WALL HEAT TRANSFER COEF...AGAIN | Carl | CFX | 2 | July 8, 2005 01:35 |
Total heat through a wall | massimo | Siemens | 0 | December 22, 2002 12:25 |