# Understanding the Marshak boundary condition (radiation)

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

 May 14, 2014, 07:18 Understanding the Marshak boundary condition (radiation) #1 Senior Member   Join Date: Oct 2013 Posts: 397 Rep Power: 18 I'm currently working on implementing a non-gray 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: With e=emissivity at the surface, sigma= Stefan Boltzmann constant and G the spectral intensity integrated over all angles. And also: (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*(2-e_w))*G_w + q_rw = -e_w/(2*(2-e_w))*4*sigma*T_w^4 --> -e_w/(2*(2-e_w))*G_w - Gamma * dG/dn = -e_w/(2*(2-e_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: 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 non-gray 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. atulkjoy likes this.

 May 23, 2014, 04:42 #2 New Member   Elia Agnani Join Date: Oct 2011 Location: Modena, Italy Posts: 5 Rep Power: 14 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); where is what I called Code: const scalarField Ep(temissivity/(2.0*(2.0 - temissivity))); and where, according to the post below 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; I have to set the emissivity value in the same dictionary Code: emissivity uniform 0.9; If I set Code: emissivityMethod solidRadiation; OpenFOAM looks for emissivity value in the radiationProperties file of the coupled solid. In the AbsorptionEmissionModel dictionary to be precise. Code: radiation on; radiationModel opaqueSolid; absorptionEmissionModel constantAbsorptionEmission; constantAbsorptionEmissionCoeffs { absorptivity absorptivity [ 0 -1 0 0 0 0 0 ] 0.0; //opaque emissivity emissivity [ 0 -1 0 0 0 0 0 ] 0.1; E E [ 1 -1 -3 0 0 0 0 ] 0; } scatterModel none; sootModel none; But here I find an emissivity in 1/m, I thought that at the wall the emissivity should have been dimensionless from 0 to 1, like in the formula Anyone can shed more light? Elia francescomarra, jherb, Tobi and 12 others like this. __________________ SnappyWiki

 May 26, 2014, 04:25 #3 Senior Member   Join Date: Oct 2013 Posts: 397 Rep Power: 18 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.

December 13, 2014, 17:29
#4
Member

Kaufman
Join Date: Jul 2013
Posts: 55
Rep Power: 12
Quote:
 Originally Posted by elia87 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); where is what I called Code: const scalarField Ep(temissivity/(2.0*(2.0 - temissivity))); and where, according to the post below 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; I have to set the emissivity value in the same dictionary Code: emissivity uniform 0.9; If I set Code: emissivityMethod solidRadiation; OpenFOAM looks for emissivity value in the radiationProperties file of the coupled solid. In the AbsorptionEmissionModel dictionary to be precise. Code: radiation on; radiationModel opaqueSolid; absorptionEmissionModel constantAbsorptionEmission; constantAbsorptionEmissionCoeffs { absorptivity absorptivity [ 0 -1 0 0 0 0 0 ] 0.0; //opaque emissivity emissivity [ 0 -1 0 0 0 0 0 ] 0.1; E E [ 1 -1 -3 0 0 0 0 ] 0; } scatterModel none; sootModel none; But here I find an emissivity in 1/m, I thought that at the wall the emissivity should have been dimensionless from 0 to 1, like in the formula Anyone can shed more light? Elia
Generally speaking, the emissivity can change depending on the wavelength. That's why there is a per unit wavelength for its unit.

 December 16, 2014, 08:38 #5 Senior Member   Join Date: Oct 2013 Posts: 397 Rep Power: 18 But a wavelength-dependent 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.

 June 19, 2018, 13:08 #6 New Member   Germilly Barreto Join Date: Jul 2016 Location: Portugal Posts: 25 Rep Power: 9 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 { type MarshakRadiation; T Ts; // Ts is the name of my temperature field value uniform 0;; } I think I have understood the parameters in the constant/boundaryRadiationProperties for the wall: Code: wall { type boundaryRadiation; mode lookup; emissivity uniform 0.8; // The emissivity of the wall value uniform 0; } I also think I have understood the parameters in constant/radiationProperties which characterize the participating media. 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 atulkjoy, Joanne, altinel and 1 others like this. Last edited by Germilly; June 21, 2018 at 13:31.

 June 27, 2018, 06:29 #7 New Member   Joanne Join Date: Aug 2017 Location: Ireland Posts: 6 Rep Power: 8 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 Last edited by Joanne; June 27, 2018 at 06:30. Reason: grammar

 June 27, 2018, 07:16 #8 New Member   Germilly Barreto Join Date: Jul 2016 Location: Portugal Posts: 25 Rep Power: 9 Hello Joanne, See my last post in the following thread: Radiation boundary conditions for flow through boundaries in openFoam I hope it can be helpful. Regards, Germilly Barreto

 June 27, 2018, 09:06 #9 Senior Member   Join Date: Oct 2013 Posts: 397 Rep Power: 18 Hello, I replied to the other thread, I hope this helps somewhat.

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Mavier CFX 5 April 29, 2013 00:00 Tuca FLOW-3D 1 April 23, 2013 12:02 CFD XUE FLUENT 0 July 8, 2010 06:49 [Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Meshing & Mesh Conversion 2 July 15, 2005 04:15 boing Main CFD Forum 1 January 6, 2002 16:53

All times are GMT -4. The time now is 09:08.