CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Solver refuses to run: Monte Carlo Radiation Model

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 9, 2012, 15:05
Default Solver refuses to run: Monte Carlo Radiation Model
  #1
New Member
 
Saumitra Joshi
Join Date: Dec 2012
Posts: 8
Rep Power: 4
Zaphod'sSecondHead is on a distinguished road
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?
Zaphod'sSecondHead is offline   Reply With Quote

Old   December 9, 2012, 17:04
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 9, 2012, 17:12
Default
  #3
New Member
 
Talita Possamai
Join Date: Sep 2012
Posts: 23
Rep Power: 4
Possa is on a distinguished road
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
Possa is offline   Reply With Quote

Old   December 10, 2012, 05:12
Default
  #4
New Member
 
Saumitra Joshi
Join Date: Dec 2012
Posts: 8
Rep Power: 4
Zaphod'sSecondHead is on a distinguished road
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



Here's the interface at the outlet:



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.
Zaphod'sSecondHead is offline   Reply With Quote

Old   December 10, 2012, 05:18
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 11, 2012, 18:57
Default
  #6
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
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?
evcelica is offline   Reply With Quote

Old   December 12, 2012, 00:25
Default
  #7
New Member
 
Saumitra Joshi
Join Date: Dec 2012
Posts: 8
Rep Power: 4
Zaphod'sSecondHead is on a distinguished road
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?
Zaphod'sSecondHead is offline   Reply With Quote

Old   December 12, 2012, 06:28
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,803
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 12, 2012, 06:39
Default
  #9
Senior Member
 
Erik
Join Date: Feb 2011
Location: Earth (Land portion)
Posts: 486
Rep Power: 9
evcelica is on a distinguished road
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.
evcelica is offline   Reply With Quote

Reply

Tags
absorber tube, cfx, monte carlo

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Would it be possible to add the radiation model into the reactinFoam solver? pajofego OpenFOAM 3 June 21, 2012 05:41
Help: Radiation model MANOJKUMAR FLUENT 4 November 24, 2005 03:45
How to use radiation model with porous model? jacky CFX 0 December 17, 2002 23:51
CFX 5.5 Roued CFX 1 October 2, 2001 16:49
definition difficulty-->DO radiation model Harry Qiu FLUENT 0 March 29, 2001 09:19


All times are GMT -4. The time now is 09:16.