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?

The emissivity is 0.9 corresponding to lab data. The simulation showed the radiative heat flux about 250W compared to convective heat flux of 160w, which is really physically impossible, with the average temperature of the surface of the heating 70C.

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

Attached is a picture for a simple model, a box with a heater inside.
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.

the only other boundary condition is the wall of the box:
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.

the external condition is accurate, the mesh is coarse in this case but i got the same confusion of the heat flux in other finer simulations. This is a steady state simulation. I also did some transient simulations, which also result in the heat flux problem.

the solve scheme:
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

How do you know? This is a very difficult thing to set accurately experimentally.

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.

We used Transys to so a series of simulations and the boundary conditions are defined depending on Transys simulation.

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.cfd-online.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.

Yes, we use different software to model a HVAC problem.
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?