Hi, I'm modelling heat flow from a central hot pipe surrounded by air, surrounded by porous insulation which has a very thin backing foil on the ouside only.

When radiation is applied to the air region and not the porous domain (montecarlo surface to surface), most of the rays emitted by the hot source get "lost" and are not absorbed by anything. I've read this means it's a setup error.

But when radiation is applied to both the air region AND the porous domain, there are no lost rays, but it treats the porous domain as transparent and deposits the radiation on the backing foil and not the surface of the insulation (which is opaque).

Is there a way of specifying the emissivity of the fluid-porous interface so that radiation is absorbed on the surface of the insulation? (whilst allowing convection through this interface.) in CFX 11 sp 1.

The radiation flux makes up a large proportion of the total heat transfer from the pipe to the outside, and having it go straight through the insulation is really screwing up my results! Any help would be much appreciated.

FYI CFX support solved this for me:

a. In the CFX PRE options, disable "automatic default interfaces" and enable "Enable Beta Features" - and make sure that constant domain physics is turned off.

b. In the neighbouring fluid domain, go to the fluid-porous interface b.c., and in "Boundary details" under "Thermal Radiation" - voila! you can set the option from "Conservative Int. FLux" to "Opaque" and specify the emissivity and Diffuse Fraction.

When solving, there are no lost rays 0.00%. However, as the interface is not a wall I can't get any "Wall ..." variables (e.g. Wall Heat FLux, Wall Radiative Heat FLux etc.). Any ideas?