Understanding the Marshak boundary condition (radiation)
I'm currently working on implementing a nongray P1 model. This also requires me to modify the Marshak BC.
The problem is that I don't quite understand how it works. I know that the radiative flux incident to the wall is: http://combust.hit.edu.cn:8080/fluen...ug/img2712.gif With e=emissivity at the surface, sigma= Stefan Boltzmann constant and G the spectral intensity integrated over all angles. And also: http://combust.hit.edu.cn:8080/fluen...ug/img2683.gif (also valid at the wall _w) The implementation uses a mixed boundary condition, that means it uses an equation of the form a*G+b*dG/dn = c. Does that mean that here this evaluates to: e_w/(2*(2e_w))*G_w + q_rw = e_w/(2*(2e_w))*4*sigma*T_w^4 > e_w/(2*(2e_w))*G_w  Gamma * dG/dn = e_w/(2*(2e_w))*4*sigma*T_w^4 I don't quite understand the code of the implementation of the Marshak BC in OF. The mixed BC fixes the value to this: http://foam.sourceforge.net/docs/cpp/form_22.png with x_p = refValue(), w=valueFraction(), dx/dn = refGrad() and x_c = value in adjacent cell. In Marshak BC refValue() is 4*sigma*T^4, refGrad() is 0 and valueFraction() is 1.0/(1.0 + Gamma*Delta/(e_w/(2*(2  e_w))). I don't understand if and how this matches the mixed equation above. Can anyone shed some light? In the nongray model, G is exchanged with G_i, and sigma*T^4 with pi*B_i, where B_i is the integral over the black body spectrum over the frequency range of the band. Does that mean I can simply replace these values in the code and it will be fine? I suppose this should work, but I would like to understand how OpenFOAM implements this. 
I think it's okay, because:
Assume that it becomes you know that from the Fluent Guide, at the boundaries is so it becomes where is the distance between face and cell center. If you explicit in the equation, you will find Here you can find the explanation of the mixed BC and it's easy to recognize that in this case because the f value (called valueFraction in OpenFOAM) can also be written as In the source code of MarhaskRadiationBC we can find Code:
refGrad() = 0.0; Code:
refValue() = 4.0*constant::physicoChemical::sigma.value()*pow4(Tp); Code:
valueFraction() = 1.0/(1.0 + gamma*patch().deltaCoeffs()/Ep); Code:
const scalarField Ep(temissivity/(2.0*(2.0  temissivity))); So I think it's ok! I have some doubts regarding the emissivity I choose in the BC, especially in case of conjugated heat transfer (chtMultiRegion solver) in OpenFOAM 2.3. If I set (in the coupled wall patch, fluid side obviously) Code:
emissivityMethod lookup; Code:
emissivity uniform 0.9; Code:
emissivityMethod solidRadiation; In the AbsorptionEmissionModel dictionary to be precise. Code:
radiation on; Anyone can shed more light? :) Elia 
Thanks, I think it's clear now how the formula translates to the implementation.
I would also agree with you that the emissivity at the surface should be in [0 .. 1]. Since the opaqueSolid radiation model doesn't do anything, I suspect it's just a different (somewhat unlucky) place to store the value in. 
Quote:

But a wavelengthdependent emissivity still is dimensionless, as it's not a density like a spectral intensity for example.
Also, the emissivity in radiationProperties is used in two different contexts in the models, which is somewhat confusing. 
Hello,
I was searching in the forum and this thread seems to be the right place to post my question. I'm modelling radiation transfer inside a pipe which contain a participating media. My problem is about the boundary condition for the incident radiation G (I'm using the P1 radiationModel). In that pipe, I have 3 boundary patches: 1) "inlet" of the pipe: Which is in direct contact with the environment 1) "outlet" of the pipe: also in direct contact with the environment 3) "wall" (cylindrical surface): Bounded by a solid diffuse surface For the wall, I'm using in the 0/G file the MarshakRadiation boundary condition: Code:
wall Code:
wall But, for the inlet and outlet, I dont know what should I do. I cannot define an emissivity for the inlet and outlet because there are no solid surface, there are only the participating media. Do you know what should I define for these two boundary conditions (inlet and outlet)? Thank you Best regards, Germilly Barreto 
Hi Germilly,
I am interested in a similar problem as yours, I am unsure which BC to use for flow inlets/outlets when implementing a radiation model. Please let me know if you make any discoveries, and I will do likewise. Kind regards, Joanne 
Hello Joanne,
See my last post in the following thread: https://www.cfdonline.com/Forums/op...tml#post696795 I hope it can be helpful. Regards, Germilly Barreto 
Hello,
I replied to the other thread, I hope this helps somewhat. 
All times are GMT 4. The time now is 11:29. 