Radiation through: glass – air cavity – glass
 

Hello all,

Here I am again to ask something about radiation using cfx5.7.1. Now I need to consider incident solar radiation effects to a double skin façade system, the physical sequences would be: Solar radiant flux (W/m^2) from solar generator is striking on an external glazing (glass with thickness 12mm) then to an air cavity, then through an internal glazing (double glazing â€" glass(6mm)+airgap(12mm)+glass(Low E, 6mm)), and then to an internal controlled environment. I have generated the solid (material glass plate) and fluid zones (air) and now I have the following questions.

1. Can I set an isotropic radiation flux on the surface of the external glass as a source (the side facing the solar generator)? If this is the case, this surface has to be a wall boundary condition, but the thermal radiation option there shows 'opaque', it seems I still need to provide a temperature (or a heat flux) and an emissivity for the boundary. The surface is not 'opaque' anymore, but I don't have other choice.

2. 'Monte Carlo' model is selected as the thermal radiation model option, should I use 'gray' or 'multiband' model for both solid zones and fluid zones? Is the scattering model necessary for this case? The radiation properties for the 'glass plate', how do I define the 'Absorption coefficient' and 'scattering coefficient'?

Any suggestions would be highly appreciated (many thanks to the previous comments from Opaque. Sorry, Opague, this time I asked more)

Regards, Yingchun

Re: Radiation through: glass – air cavity – gl
 

Any comments here? eagerly waiting responses from you experts.

regards, yingchun

Re: Radiation through: glass – air cavity – gl
 

Dear Yingchun,

Have you had a look at the Heating and Ventilation tutorial? There is an example showing where to setup the solar radiation condition. The example uses directed (collimated) radiation..

CFX does not support semi-transparent external boundaries, but you add these external radiation influences via sources. They can also be a function as frequency/wavelength as well.

When setting up an external directed radiation source, be careful with the External Refractive Index setting. If you do not set it, the rays is taken without refraction through the first boundary of the solid.. Set/Unset it and you will be able to see what I mean..

Again regarding modelling, it is up to you what you want to do.. In general, radiation solar calculations are done with two bands. More bands usually do not bring additional bang for the buck..

Regarding Gray, and Multiband models. CFX does not support mixing the models across a domain interface, that is, if one side is Gray, the other side must be the same as well. Otherwise, you will get an strange error message..

Properties are set in the same spot for fluids and solids: materials tab.

Good luck, Opaque

Re: Radiation through: glass – air cavity – gl
 

Thank you, Opaque, i am afraid I didn't find the 'heating and ventilation tutorial', would you please let me know where i can find it? I use the command line 'cfx5help' and i can access all the tutorials listed there, but it seems the tutorial you mentioned is not there.

Thank you for your help again

Regards, yingchun

Re: Radiation through: glass – air cavity – gl
 

It is called Air Conditioning Simulation, or tutorial 17 in ANSYS CFX 10.0.. It may be a different number in 5.7.1

Look for the Window boundary section..

Opaque..

Re: Radiation through: glass – air cavity – gl
 

Hi Opaque, Thank you for your information. Just found it, actually, the same number. wasn't aware this is the title. I've also read some informaiton - cfx5 best practices guide for HVAC - which gives some suggestions on how cfx deals with direct solar radiation.

You are really helpful, thank you very much (no further question for now)

Regards yingchun

Thermal radiation through single and double glass using ansys-fluent
 

Pls,does anyone have an idea of how to go about modelling solar thermal radiation through air-glass-air and air-glass-air-glass-air.

I have just started using e ansys fluent software but things seems not to be going of fine.


Pls help

There are tutorials on this in the CFX documentation. But if you are using Fluent you are on the wrong forum - this is the CFX forum.