Simluate smoke indoor (Smoke visibility)

[z3351922]

hi~
I try to do the smoke visbility on Autodesk CFD simulatio, but i can't generate the smoke in CFD
i follow the GuideLine, but it is still not success.
Can anyone help me here ???

I created a house with two holes. One is on the side, One is on the ceiling.
In the middle of the house there is a box where the fire generated.

material
Volume inside the the house is air. I set it to be variable.
The wall of the house is brick. The box in the middle is made by hardwood.

Boundary Condition
Box: Scale = 1, Heat Generation = 2000W 
Air: Film Coefficient = 5 W/m2/K, Ref. Temp.  = 19 Degree
Hole on Ceiling: Volumetic Flow Rate = 50 L/s,
Hole on Side : Pressure = 0Pa , Temperature = 20 Degree.

Solve:
Set Smoke Visibility on
Heat Transfer on
Specific Extinction Coefficient = 21000
The sign visibility constant characterizes = 3

combustion particulate yield = 0.08
Diffusion Cosfficient  = 16 mm^2/s

 
Solution :
i set the output quantity is Scalar

However, i cannot see the smoke in the CFD.
Can Anyone help me
I want to create the view like the one in the Guideline. Smoke visibility

[Jon.Wilde]

Set Scalar = 0 at the inlet and also as an Initial Conditon of Scalar =0 to the entire volume.

Is the Scalar = 1 BC only on the top surface of the fire yes?

What material is the fire? We typically use a highly conductive and 100% open resistive region. It is also advisable to

1. Have a solid material around the sides of the fire, this ensures the flow passes through it from bottom to top
2. Have a gap beneath the fire for air to pass into

Be sure to run this transiently also.

[z3351922]

The fire is on the hardwood.
i set the the scalar on the top surface of hardwood
it is around by four brick walls
do i need to add heat generation on the hardwood?
any suggestion for the values of heat heneration and the diffusion coefficient?

[Jon.Wilde]

OK.

Please follow what we recommend and use a resistance (with 100% open area) rather than hardwood - include a gap beneath it also.

Yes, you will need a heat generation, this value totally depends on what you are modelling, it could be thousands of watts.

Your diffusion coeff looked OK as you originally had it set.

[z3351922]

Thanks for the replied

I want to ask why we are using resistance instead of solid for burning?

Besides, when i import the model from Autodesk revit to the Simulation, the coordinate direction of the model in CFD is changed.
Are there any ways to correct the direction.
Now the bottom side of the model becomes the back side in CFD.
How to correct it? Does it affect the result? 

Now, I set the material is resistance and the Scalar only on the top surface of the resistance. Is that correct?

Set Boundary Conditions:
inlet: Pressure = 10Pa, Temperature = 25 degree, Scalar = 0
Outlet : Velocity exhaust 1m/s
Wall: Brick, Film Coefficient = 10 W/ m^2 / K, Ref Tem = 25 Degree
Resistance: Scalar =1 (Only on the top face), Heat Flux = 100k W/m^2 (Only on the side faces), Heat Generation = 5000W 
The Soild arould the Resistance: I set it to be Aluminium.  Film Coefficient = 15 W/ m^2 / K, Ref Tem = 25 Degree

Initial Conditin:
Air Volume: Scalar = 0

Solve:
Solve By Transient
Set Smoke Visibility on
Heat Transfer on
Specific Extinction Coefficient = 21000
The sign visibility constant characterizes = 3

combustion particulate yield = 0.08
Diffusion Cosfficient  = 16 mm^2/s
Garvity : Earth ( 0 , 0 , 0) (Not Sure if it is correct)

When you said we need a gap beneath the fire for air to pass into. Do we need to drill a hole on the base connection to the resistance?

Now i still cannot simulate a correct smoke distribution in the model.
I attach the picture of my result i simulated and the my CFD simulation.
Are there any mistakes in my setting?

[Jon.Wilde]

Hi, I have added some comments below:

I want to ask why we are using resistance instead of solid for burning? 

It represents a fire better, the air can pass through it and gain large amounts of heat as it does.

Besides, when i import the model from Autodesk revit to the Simulation, the coordinate direction of the model in CFD is changed.
Are there any ways to correct the direction No, they should match. You can work around this just by setting the correct gravity direction in CFD though
Now the bottom side of the model becomes the back side in CFD.
How to correct it? Does it affect the result? 

Now, I set the material is resistance and the Scalar only on the top surface of the resistance. Is that correct?  Yes

Set Boundary Conditions:
inlet: Pressure = 10Pa, Temperature = 25 degree, Scalar = 0
Outlet : Velocity exhaust 1m/s
Wall: Brick, Film Coefficient = 10 W/ m^2 / K, Ref Tem = 25 Degree
Resistance: Scalar =1 (Only on the top face), Heat Flux = 100k W/m^2 (Only on the side faces), Heat Generation = 5000W  The heat flux should be applied to the volume, so switch from surface selection to volume and apply to the 3D resistance, not surfaces. The scalar is fine on the surface though.
The Soild arould the Resistance: I set it to be Aluminium.  Film Coefficient = 15 W/ m^2 / K, Ref Tem = 25 Degree

The ONLY internal surface BC you should have is the scalar = 1 on the top of the fire, delete all of these other film coeffs, CFD will calculate it for you

Initial Conditin:
Air Volume: Scalar = 0

Solve:
Solve By Transient
Set Smoke Visibility on
Heat Transfer on
Specific Extinction Coefficient = 21000
The sign visibility constant characterizes = 3

combustion particulate yield = 0.08
Diffusion Cosfficient  = 16 mm^2/s
Garvity : Earth ( 0 , 0 , 0) (Not Sure if it is correct) Set a 1 (or -1) in the gravity direction and also ensure you have Air set to Variable. You need to have both of these set so that the hot air will rise

When you said we need a gap beneath the fire for air to pass into. Do we need to drill a hole on the base connection to the resistance? No, just have it offset from the floor so that air can pass underneath and be drawn though the resistance.

Now i still cannot simulate a correct smoke distribution in the model.
I attach the picture of my result i simulated and the my CFD simulation.
Are there any mistakes in my setting?