Simple radiation validation problem
5 Attachment(s)
Hi All
I am trying to solve a very simple radiation case in order to validate OpenFoam's radiation model/s, so far with little success. The case I'm trying to solve is a 2D square enclosure (1m x 1m):
I have attached the following:
Qr on the leftWall should be uniform across the whole surface equal to 5.67, which I am able to get with the custom solver, but not with the buoyantSimpleFoam solver (for some reason the thermal conductivity in the energy equation has an effect on Qr). Qr on the rightWall should give a areaweighted sum of 2.3474, in paraFoam I get an areaweighted sum of 0.6103. I am unable to get the correct Qr for the right, top and bottom surfaces. I hoping that this is the case of me missing something fundamental so any comments / advice would be useful :D 
Can someone please explain to me how and where these coefficients (in the radiationProperties file) play a role in the radiation models:
Code:
absorptionEmissionModel constantAbsorptionEmission; 
Quote:

Hello, Logan Page.
The spherical harmonic approx. method (P1) gives me 8.47 [W/m2] and 2.79 [W/m2] for q_left and q_right correspondingly. The discrete ordinates method gives me 5.67 [W/m2] and 2.31 [W/m2] for q_left and q_right correspondingly. This result is very close to theoretical one. I haven't used viewFactors model yet. If you're still interesting in this stuff, I can share test case here. 
hello,
You can not use P1 model with an empty cavity, since P1 model is for optical thick media (a*l >1), with a= absorptivity and l = carac. length DO and viewfactor method should work however. regards, olivier 
1 Attachment(s)
Hi
Thanks for the feedback. I was able to get the theoretical results using the DO method by setting "absorptionEmissionModel" to "none" in the "radiationProperties" file. I was also able to figure out the theory and 90% of the implementation thereof in OpenFOAM for the DO method through the use of the book by M. Modest (Radiative Heat Transfer, 3rd Edition) However for the life of me I cannot figure out why there is an additional source radiation term implemented for the DO method in OpenFoam. For a participating, nonscattering, medium the governing RTE is given by: http://www.cfdonline.com/Forums/att...1&d=1380536642 However in OpenFOAM there is an additional source term that has been added: Code:
IiEq = For a "constantAbsorptionEmission" model "ECont(lambdaI)" is simply the "E" value specified by the user in the "radiationProperties" file. For a "greyMeanAbsorptionEmission" model "ECont(lambdaI)" is "EhrrCoeff * dQ" where again "EhrrCoeff" is specified by the user in the "radiationProperties" file. 
Quote:
could you kindly share your test case ? I am facing the same problem and I want to learn a little about how to set up radiation from your case. thank you very much. 
Quote:
I was a bit confused by this when I first saw it too  as you correctly say, only the first three terms appear in the theoretical RTE. However this is a numerical implementation and I believe the reason for the E parameter in the absorptionEmissionModel is to allow the user the choice of defining the emissive power of the gas directly (W/m3), rather than via the gray gas relation (emissivity * planck function). This would be useful if one wanted to apply a radiative source term that does not vary in proportion to the Planck function. S 
I Need Help
1 Attachment(s)
Hello all,
I am new to this forum. I really need your help to solve my problems in running openfoam. attached is my geometry. There are 5 rows of vanes in front of an intake channel. I have produced my geometry, but I think it is not correct. Does any body know, how I can define the water surface in my geometry? I want to consider it as rigid lid. Then my flow in the channel in turbulent, and I want to use kepsilon turbulent model for the simulations. Any help is really appreciated. 
Dear Friends,
In the example of validation discussed, as you would to include the ViewFactor model? What files should include? I appreciate everyone's attention. 
Quote:
I am eager to know as well. 
Dear Logan page,
I am new to the OpenFOAM and hence may sound stupid! Could you pls tell me how did you manage to set up your problem with no convection and conduction ( Conduction i can understand as no solid body present). and if I want to consider convection with radiation what necessary changes i have to make?? Thanks in advance! Regards, Amit Dhage 
Quote:
However, I'm not sure conduction really is deactivated, since the thermophysicalProperties values give mu and Pr, which I assume are used für thermal conductivity. Anyway, this should be quite small and probably has little influence on the solution (maybe the reason vor ARTems deviation from the exact soluton). Quote:

Quote:

All times are GMT 4. The time now is 02:05. 