Hooray! CFD-Online is back... Thanks to the support team!!!

Dear experts, I do my first radiation simulation with Monte Carlo in a rectangular channel consisting of different parts & materials (e.g. ZnSe window, metal and ceramic walls, ...). The goal is to find out the radiation from the adjacent channel walls to a specified wall surface area (target plate). Air within this channel is treated as transparent medium and since convection is not considered (in a first approach) only the solid is modeled & meshed, i.e. there is no fluid domain. I've done some test runs with different parameters (emissivity, temperature BC, # of histories) to see what happens. In CFX-Post I visualize the "Wall Irradiation Flux".

Here are my questions:

1) Is it possible to define a domain (window) as a transparent solid? With Monte Carlo (Surface to Surface) only opaque solids are supported. Boundary Details > Thermal Radiation > Option: ... I used to model the ZnSe window (transmittance >90%) as a opening... Any suggestions how to overcome this problem? In the help manual "Radiation Properties" it is described that transparent media has an absorption coefficient and scattering coefficient of zero.

2) Is a (fine) mesh necessary at all or just a (1part-1element) mesh converted directly from the raw blocking? With this I would like to know whether the generic rays/photons in MC are dependent on the nodes or created by random within the mesh-element. The fact that there is a "coarsening control" tells me that the number of elements is relevant but I'm not sure...

3) Is the # of histories defined per domain-mesh-element or just per domain? Here I guess it is per domain but then in question 2) the number of mesh elements in a domain is not important for pure radiation modeling. I've defined a domain for each part of the channel.

I hope someone can give me an advise. Thanks in advance!

Zoran

Here is an update of my "progress":

Since my contour plot seemed to be unreliable (very speckled, even with 1 billion # of histories!), I refined my mesh in ICEM by a factor of 2 (element edge). The total number of elements has consequently increased by a factor of 4 (--> around 750'00 nodes/quads). Running now the Monte Carlo on CFX, with fixed uniform temperature BC, provides a worser contour plot!! For the "Wall Irradiation Flux" I see the plot divided in small squares (approx. 10x10 mesh elements). I increased the # of histories to 10e6 but no improvement.

...then I reduced the "Target Coarsening Rate" from 64 to 4. With this the squares disappear and the speckled-like contour plot is obtained again but the Min/Max values are still distinct.

Is there an optimal ratio between mesh-element size and # of histories?

Dear Zoran,

Here are my comments on your different points:

1) Do you need a transparent solid, or a transparent boundary? You can use Monte Carlo within a solid domain, and set the transfer mode to Surface to Surface (assumes the material is transparent). The boundaries are still opaque.

2) I do not understand you question about the mesh. However, the coarsening controls are there to coarsen the volumetric mesh (and implicitly the boundary faces as well). The histories start at boundaries (random location within the faces), and at volumes (if using the participating media transfer mode). When using the Surface to Surface transfer mode, the faces on the boundary are not coarsened at all.

3) The number of histories is per "full conjugate radiation problem". That is, if several domains are involved in the radiation calculation, they form a single radiation problem. Always keep the number of histories setting equal in all domains that are in the same "group". The number of elements in the domain (you mean volume) is not important for Surface to Surface, but it is very important for Participating Media.

Hope this helps,

Opaque

Dear opaque,

first I would like to thank you for your help! Your comments are always very precious. It seems to me that there are not so many "radiation experts" out there, or they don't use CFX. Maybe my posts are not precise enough or to long?!

1) Since I model my rectangular channel as a 2D mesh (1 layer thick) without mesh between walls, the window that needs to be set as transparent is defined as a domain having a boundary. So I guess my answer to your 1st question is: transparent boundary.

With this I want a fraction of the photons (proportional to the transmittance >90%) to leave my channel when they hit this window. The other part is reflected towards the other channel walls.

2)&3) I don't have any participating media (fluid) in the channel. Only the inner wall surfaces are involved in the radiation simulation.

Lets say I have a copper plate (100x100 mm^2) as a part of a wall, having its own (2D + 1 layer) mesh. Is it better to mesh the plate to get 100x100 small elements or just 1x1 single big element?

According to your explanations: "The histories start at boundaries (random location within the faces)" and "The number of elements in the domain (you mean volume) is not important for Surface to Surface" the mesh element size is not important for s-t-s radiation. Hence, refining the mesh doesn't improve the results but increasing the # of histories does. Agree?

Zoran

Dear Zoran,

CFX does not have a transparent "external" boundary condition. However, if you are modeling heat transfer between 2 domains: a solid and fluid, the boundary between them is treated as a domain interface.

For a domain interface, you can activate the thermal radiation model on both domains and set the boundary condition at the interface boundaries as Conservative Interface Flux. The solver will compute the proper transmission, refraction, reflection based on the refractive indexes on each side of the interface. The main assumption is that the boundary is smooth, not modeling of any kind of film; therefore, Fresnel's equation prevail.

In CFX 11.0 you cannot enforce the transmissivity at the boundaries. Are you modeling some kind of surface treatment, roughness, coating on the boundary?

Be careful, when you refer to the mesh do you mean the volume mesh, the surface mesh, or both. The surface mesh is always important; otherwise, you will never get the correct distribution due to the radiation from other boundaries.

Hope the above helps,

Opaque

Dear opaque,

Since my last post I've made some progression. The Monte Carlo simulation is now running and I get some good results. In addition I run also Discrete Transfer simulation in order to compare and use it as validation.

I still have to figure out how to set one boundary condition as 90% transparent (ZnSe window of my channel). As you wrote there is no possibility to set the transmissivity. Only opaque surfaces are allowed in MC.

Is there a way to work around???

The properties of the ZnSe window are:

T = 380 K, transmissivity = 0.90, emissivity = 0.07, reflectivity = 0.03 ---> sum = 1.00

The emitted radiation is therefore:

q' = emiss * sigma * T^4

= 0.07 * 5.67051 * 10^-8 * 380^4

= 82.77 [W/m^2]

I tried to do the following:

The surface is opaque and gray (emiss = 0.97) and the idea is to define a "dummy temperature" such that the emitted radiation is equal to q' = 82.77.

q' = 0.97 * sigma * (T_dummy)^4 --> T_dummy = 197 K

With this, almost all irradiation onto the window is absorbed and much less is emitted such that the difference between absorbed and emitted radiation is virtually transmitted.

My overall goal is to determine the radiation from the channel walls trough the window.

Any comment and help is greatly appreciated!

Zoran

... or can I use a (negative) source term in the window boundary condition as a function of the "Wall Irradiation Flux" (WIF)? But then the source boundary condition is a function of a result (WIF) which is not known when starting the solver.

How to define the expression?