Solver refuses to run: Monte Carlo Radiation Model
 

Hi!

I'm trying to simulate radiation on a Copper absorber tube surface using the Monte Carlo Radiation model. The geometry consists of two models: the inner water body, and the copper tube. Both have been meshed using the CFX physics tetra patch conforming method.

Few details:

1.1 Domain: CopperTube

- Participating Media Transfer Mode
- # of Histories: 10000
- Spectral Model: Gray
- Scattering Model: Isotropic

1.1.1 Boundary: Outer CopperTube Wall
- Heat Flux: 30000 W/m2 (Assumed)
- Emissivity: 0.05 (Polished Cu assumed)
- Diffuse Fraction: 0.01
1.1.2 Domain Interface: CopperTube and Water
- Heat Transfer: Conservative Heat Flux
- Emissivity: 0.05 (?)
- Diffuse Fraction: 0 (?)

1.2 Domain: Water

- Thermal Radiation: None
- Heat Transfer: Thermal Energy

1.2.1 Domain Interface: Water and Coppertube
- No-slip, Smooth Wall
- Heat Transfer: Conservative Interface Flux
1.2.2 Inlet, Outlet Conditions (not relevant here)

1.3 Default Fluid Solid Interface

- Interface Model: General Connection, Automatic Mesh Connection
- Additional Interface Model: Conservative Interface Flux
- Interface Model: None

The solver exits at the first iteration saying: "Too many iterations for MC Model. Reasons: (a) Highly reflective walls, (b) Small absorption coefficient, (c) Symmetry Planes are too close, (d) Geometry Specs error"

My questions are:

1. Is it okay to mesh the copper tube using CFX as default physics? I couldn't find any other way to mesh it.

2. What do the parameters Emmisivity and Diffuse Fraction mean at the Fluid-Solid Interface? What values would you guys recommend for Copper?

3. Having specified heat transfer conditions at the interface boundaries in both the CopperTube and Water domain, do we need to check the "Additional Interface Model" to 'Conservative Interface Flux' in the Default Fluid Solid Interface?

Could you guys please help me identify the problem?

1. Yes.
2. This is basic radiation modelling - you need to read up on this stuff if you are going to do radiation modelling. And the values you use depend on your model: If your pipes are smooth and shiney then a low emissivity and low diffuse fraction makes sense, if they are dull or corroded the high emissivity and high diffuse fraction make sense.
3. No, I do not think so.

Hello,

It seems to me you're making a few radiation modelling mistakes.

1 - Copper is a opaque material in the thermal radiation spectrum. So it should not be treated as a participating media as you have done.

2 - If you use a participating media for the copper you cannot set emissivity and diffusion fraction.

3 - You've set water domain to have no thermal radiation. That makes no sense. Don't you want to solve the radiation exchange between copper and water??

4 - The emissivity and diffusion factor in the fluid-solid interface surface are the only ones you should have set. They define the radiation exchange problem.

So, summarizing: your model definitions are all messed up.

I recommend you take a little time to study about radiation energy transfer between solid and fluid before continuing with your problem.

If you post a picture of your problem I can probably help you set the model right. But you really should try to understand all models you are solving to be able to judge your results.

Regards,
Possa

Thank a lot for the response, Mr. Ghorrocks and Mr. Possamai!

I was a little confused back then. I looked up some text, and redefined the problem as follows:

1.1 Domain: Copper

- Participating Media Transfer Mode
- # of Histories: 50000
- Spectral Model: Gray

1.1.1 Boundary: Outer Wall

- Boundary Source: Isotropic Radiation Flux of 14000 W/m2
- Opaque Boundary, Emissivity = 0.05, DF = 0.1

1.1.2 Domain Interface: CopperTube and Water
- Heat Transfer: Conservative Heat Flux
- Thermal Radiation: Conservative Heat Flux

1.2 Domain: Water

- Thermal Radiation: Monte Carlo, 10000 Histories
- Heat Transfer: Thermal Energy

1.2.1 Domain Interface: Water and Coppertube
- No-slip, Smooth Wall
- Heat Transfer: Conservative Interface Flux
- Thermal Radiation: Conservative Heat Flux
1.2.2 Inlet, Outlet Conditions (not relevant here)

1.3 Default Fluid Solid Interface

- Interface Model: General Connection, Automatic Mesh Connection
- Additional Interface Model: None

http://i.imgur.com/q4EqC.png?1

Here's the interface at the outlet:

http://i.imgur.com/tdMHF.png?1

Solver Control:

Liquid timescale: 20 secs
Solid Timescale: 100 secs
Topology Estimation Factor: 1.2

I ran the Solver, and after around an hour, it displayed this:

ERROR #666000005 has occurred in subroutine WALK.
| Message:
|
| Too many iterations while using Monte Carlo.
| This may possible be due to:
| 1 - Highly reflective walls
| 2 - Small absorption coefficient
| 3 - Symmetry planes are too close, i.e. 2D geometry
| 4 - Geometry specification error

Please help..

EDIT: The tube thickness is 1/8 inch.

Looks like you can use the Discrete Tansfer model for this rather than Monte Carlo. If you only really need view factors and the path is not important then this will be far easier and much faster.

Have you determined if radiation in the pipe will actually be significant? I don't know how much flow there is in the pipe or at what temperature, but looking at your geometry I would think convection would dominate and radiation in the pipe would be pretty negligible?

Thanks for the post, Erik and Ghorrocks!

I agree with you, Eric. Actually, what I am trying to simulate is solar radiation input on the copper pipe that would result in it being heated up.
For that, I have now modified my design andcreated a layer of air around the tube. But the problem is, that in the CFX-Pre setup, it detects both the medium inside the tube and outside it as the same, i.e., if I define the inner region as "Air at 25C", the outer region automatically gets defined as "Air at 25C".

Any solution?

If you are modelling solar heating then why not just model it as a heat source on the outer wall of the solid domain? No need for an outer air domain.

Like Glenn says, just add an equivalent heat source to the outer wall, and the skip radiation modeling.
Also for future reference you have to go to something like: options >> general >> beta features >> and uncheck the "constant domain physics" box if you want to do more than one type of fluid.

computational problems
 

2 things:
- I am facing a similar problem I suggest you to use a coarser mesh as the error might be due to insufficient computetional power. In my case it works with a coarser mesh
- radiation source: you can set a radiation source in the boundary condition, I suggest you to have a look to the ansys HVAC tutorial