Radiation model problem
Hi everyone. When I use CFX these days to do a HVAC(Heating Ventilating And Air Conditioning) simylation for a small room, one thing always confuses me. When I set a fixed heat flux on a heating in the room and activate the radiation model, I find that radiative heat flux from the heating always takes a great part of the total fixed heat flux from the heating(about 50% to 70%),and the convective heat flux takes a smaller part. The average temperature on the surface of heating is about 70C, according to our experiment the ratio of radiative and convective heat flux of the heating is about 3:7 or 2:8.
Is it because of the radiation model? I used both Discrete Transfer and Monte Carlo, almost the same result. 
It could possibly be because of accuracy in the model, but both Discrete transfer and Monte Caro should work for this application when correctly set up.
My guess is you have not set the radiative and convective boundary condition up correctly. Is the emissivity correct? 
Quote:

The problem is likely to be in the way you have implemented the heater. How have you done this? Please show an image.

1 Attachment(s)
Quote:
the boundary condition of the heater: BOUNDARY: Heater Boundary Type = WALL Location = HEATER BOUNDARY CONDITIONS: HEAT TRANSFER: Heat Flux in = 366.82 [W m^2] Option = Heat Flux END MASS AND MOMENTUM: Option = No Slip Wall END THERMAL RADIATION: Diffuse Fraction = 1. Emissivity = 0.9 Option = Opaque END WALL ROUGHNESS: Option = Smooth Wall END END END 
Is the flux truly uniform? What about the other wall conditions? What about the flow generated? The heat flow from the heater is coupled to the heat absorption from the rest of the room so you cannot consider the heater in isolation.

2 Attachment(s)
Quote:
BOUNDARY: Wall Boundary Type = WALL Location = WALL BOUNDARY CONDITIONS: HEAT TRANSFER: Heat Transfer Coefficient = 1.887 [W m^2 K^1] Option = Heat Transfer Coefficient Outside Temperature = 10 [C] END MASS AND MOMENTUM: Option = No Slip Wall END THERMAL RADIATION: Diffuse Fraction = 1. Emissivity = 0.9 Option = Opaque END WALL ROUGHNESS: Option = Smooth Wall END END END DOMAIN MODELS: BUOYANCY MODEL: Buoyancy Reference Density = 1.205 [kg m^3] Gravity X Component = 0 [m s^2] Gravity Y Component = g Gravity Z Component = 0 [m s^2] Option = Buoyant BUOYANCY REFERENCE LOCATION: Option = Automatic END END DOMAIN MOTION: Option = Stationary END MESH DEFORMATION: Option = None END REFERENCE PRESSURE: Reference Pressure = 1 [atm] END END the pictures attached shows the temperature distribution with z=0.2m and the velocity vectors in the middle of the box. 
Is h=1.887 at 10C really accurate for the external walls? Are you running this steady state or transient? What differencing scheme?
You mesh looks very coarse on your vector plot. 
Quote:

Quote:
FLUID DEFINITION: Fluid 1 Material = Air Ideal Gas Option = Material Library MORPHOLOGY: Option = Continuous Fluid END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Option = Thermal Energy END THERMAL RADIATION MODEL: Option = Discrete Transfer Radiation Transfer Mode = Participating Media SCATTERING MODEL: Option = None END SPECTRAL MODEL: Option = Gray END END TURBULENCE MODEL: Option = SST BUOYANCY TURBULENCE: Option = None END END TURBULENT WALL FUNCTIONS: Option = Automatic END END END INITIALISATION: Option = Automatic INITIAL CONDITIONS: Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS: Option = Automatic with Value U = 0 [m s^1] V = 0 [m s^1] W = 0 [m s^1] END RADIATION INTENSITY: Blackbody Temperature = 20 [C] Option = Automatic with Value END STATIC PRESSURE: Option = Automatic END TEMPERATURE: Option = Automatic with Value Temperature = 20 [C] END TURBULENCE INITIAL CONDITIONS: Option = Low Intensity and Eddy Viscosity Ratio END END END 
Quote:
Have you done a mesh refinement study? I suspect you will need to go quite a bit finer before you get mesh independance. And a flow like this is unlikely to be steady state in my experience. It almost certainly has large scale fluctuations which a turbulence model cannot capture. 
Quote:
the mesh was implemented in Tetra meshing with Hexa core and Prism layers. Is it because of the mesh for the heat flux problem? If so ,can you give me some advice on how to do HVAC mesh? 
So you are validating your CFX simulation against another simulation package?
The question here is not specific to the heater, but a more general one of simulation accuracy. This FAQ gives some tips (http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F) but is really just a starting point. The issue of accurate CFD simulations is a complex and detailed area and has been the life's work of many talented researchers  so it is unlikely I can sum it up in a forum posting. But one researcher I can highly recommend is the work of Roache, particularly his textbook "Computational Fluid Dynamics". This work really brought together many issues of CFD accuracy (well, at least for me it did) and I suggest you have a look at it to understand the issues involved in accurate CFD simulations. 
Quote:
There is an air conditioning case in the CFX tutorials, and I also got several cases of HVAC simulation using CFX, as well as meshing using CFX mesh(although i use ANSYS ICEM CFD). I meshed and modelled according to the tutorial so i think this is not a big problem for my case. Plus i really don't have so much time to study CFD so carefully although i really don't wanna say this.. 
The tutorials show you what buttons to press to get a simulation to run. They do not show you what you should do to get an accurate simulation. In particular the meshes they use are far too coarse for accuracy and are chosen to get the model to run quickly. So do not use the tutorials as a guide of how to set up an accurate simulation.
If you are validating against another CFD code you should be able to use exactly the same boundary conditions it used. For instance make sure the h value quoted is not an averaged value. The simulation you are doing is not trivial and getting accurate answers will require some work. 
HVAC using Fluent/Ansys
Hi All,
I have been coming here for some weeks now and i have always been impressed by some of the response of some intelectuals here.Pls,i have a question to ask regarding my dissertation. I am presently working on HVAC,where i need to include double glazed window(Design modeller>sketching of the window in 2D on the plane>concept>line from the sketch plus frozen enhanced. Pls can someone advise me how to make it double glazing because wht i have shown above is for single glass window. Hope to hear from you soon,as i need to hand in my dissertation soon. Thanks 
Firstly, welcome to the forum.
Secondly, please post new questions as a new thread. Do not confuse other threads by changing the topic. To answer your question: I am not sure what you are asking, but the CFX tutorials show how to model CHT materials and how to set them up. Is this what you are asking? 
All times are GMT 4. The time now is 07:33. 