last revised 19/08/2010
1.1 What is FLAIR ?
1.2 What FLAIR can do
2.2 Accessing the FLAIR on-line help
2.3 A simple example
2.3.1 Problem description
2.3.2 Setting up the model
2.3.3 Running the Example
2.3.4 Viewing the Results with VR-Viewer
2.3.5 Printing from VR
2.3.6 Summary
3.1 The HVAC specific object types
3.1.1 Diffuser
3.1.2 Fire
3.1.3 Jetfan
3.1.4 Spray-head type
3.1.5 Person
3.1.6 People
3.2 The HVAC-specific objects and their default attributes
3.2.1 Cabinets subdirectory
3.2.2 JETFANS subdirectory
3.2.3 Living subdirectory
3.2.4 PERFPLAT subdirectory
3.3 How to import the HVAC objects
3.3.1 Using the Object Management dialog box
3.3.2 Object attributes
3.3.3 Exporting Object
3.3.4 Object sizing, scaling and
positioning
3.3.5 Object Colouring and Rotation
options
3.3.6 Import custom geometry
4.2 System curve
4.4 Comfort Index
4.4.1 Dry resultant temperature (TRES)
4.4.2 Predicted mean vote (PMV)
4.4.3 Predicted percentage dissatisfied (PPD)
4.4.4 Draught rating (PPDR)
4.4.5 Predicted productivity loss (PLOS)
4.4.6 Mean age of air (AGE)
FLAIR is a special-purpose program for Heating, Ventilation and Air Conditioning (HVAC) systems that are required to deliver thermal comfort, health and safety, air quality, and contamination control. FLAIR provides designers with a powerful and easy-to-use tool which can be used for the prediction of airflow patterns, temperature distributions, and smoke movement in buildings and other enclosed spaces. For example:
Figure 1.1 The temperature distribution in Hackney Hall
Figure 1.2 The temperature distribution in a computer room
Figure 1.3 Temperature contours of the hot gases from a fire on a plane through the central space of a multi-storey car park (all temperatures above 100 degree C are shown in red)
Figure 1.4 Wind test over Melbourne cricket ground
As seen from above examples, FLAIR can be used during the design process to detect and avoid uncomfortable air speeds or temperatures. In addition, it can predict the effects of any gaseous pollutant, helping to achieve safe design of buildings, underground systems etc. It can also be used by various regulatory bodies and safety consultants.
FLAIR provides a state-of-art Virtual Reality User Interface for rapid model creation and visualisation of the results, including various thermal-comfort parameters. Little CFD knowledge is therefore required to operate FLAIR or to understand this guide.
1.2 What FLAIR can do
FLAIR allows the simulation of systems which are two- or
three-dimensional in space, and either time-dependent or steady.
All the functions that are required to create a FLAIR model, to solve the problem, to examine the results and On-line help can be accessed through a single integrated FLAIR-VR interface.
This chapter gives instructions for starting the FLAIR application. Following a simple example, you will use FLAIR to set up a problem, solve the problem and view the results. This is only a basic introduction to the features of FLAIR. Working through more tutorials described in Chapter 6 will provide a more complete demonstration of the program's features.
2.1 The Modes of FLAIR operation
The FLAIR pre-processor has several modes of operation. These are:
The 'VR-Environment' provides a graphical working environment in which users can run the FLAIR modules they wish, including Satellite, VR-Editor, Solver and VR-Viewer. It also provides mechanisms for:
The 'Satellite' mode is suitable for experienced users who do not wish to use the file-handling facilities provided by the VR-Environment, and are happy to run the individual modules from the system command line. The input Q1 file is read, and the EARDAT file for Earth is written after an (optional) interactive PIL command session.
For details about how to start FLAIR in the Satellite mode, the user is referred to PHOENICS document, Tr326. This document uses the FLAIR VR-Environment for this simple example.
2.2 Accessing the FLAIR on-line help
The Help button on the Help menu leads directly to this document and other documentation section of POLIS (PHOENICS On-line Information system) as shown below.
In FLAIR VR, information on the various hand-set control buttons can be displayed when the cursor is held stationary over any relevant control button. For example, when the cursor is held stationary over 'Menu' button, 'Domain attributes menu' will be displayed as shown below.
The following additional on-line help is available in the main menu of the FLAIR VR-Environment.
Click on the 'Help' button in the top menu for help on the main menu.
Click on the '?' in the top-right corner of any dialog box, then click on any input window or button to get information on the parameter which is set in it.
For example, if you want to obtain the information about Energy Equation,
'Temperature', click on the '?', 
in the top-right corner of any dialog box, then click on
'Temperature' button
, the following information will be displayed:
Figure 2.1 shows the geometry of the example. The problem solved involves a room containing an air opening, a vent, a standing person, floor and walls held at a constant temperature. The room is 5m long, 3m wide, and 2.7m high. The opening measures 0.8 m x 1.0 m and introduces a cold air jet into the room to ventilate it. The vent is 0.8 m x 0.5 m. The interaction of inertial forces, buoyancy forces, and turbulent mixing is important in affecting the penetration and trajectory of the supply air.
Figure 2.1 The simple example
We will take the following steps to set up the model:
The remaining sections provide step-by-step instructions on how to set up the model.
2.3.2 Setting up the model
Figure 2.2a The 'File' menu Figure 2.2b 'Start New case' dialog
The FLAIR VR-Environment screen shown in figure 2.3 below should appear, which consists of two components: the Main window and the control panels (on the right).
Figure 2.3 The FLAIR-VR environment
FLAIR will create a default room with the dimensions 10m x10m x3 m, and display the room in the graphics window.
You can rotate, translate, or zoom in and out from the room by clicking the 'Mouse' button on the movement control panel and then using left or right mouse buttons.
Figure 2.4 Resize the default room to 3mx5mx2.7m on the control panel
on the toolbar and then click "Fit to window" on the
pulldown.
The resized room shown in figure 2.5 will appear on the screen.
Figure 2.5 The resized room
2,3.4 Adding objects to the room
a. add the first object, which will act as a person in the room.
Figure 2.6 The Object management dialog Box.
Figure 2.7 The Object specification dialog box
Figure 2.8 The PERSON's attributes panel
Set:
Body width: 0.6 m
Body depth: 0.3 m
Body height: 1.76 m
Figure 2.9 The standing man's attributes
Click on 'OK' to return to 'Object Specification' dialog box.
X: 1.5 m
Y: 2.0 m
Z: 0.0 m
Click on 'OK' to close the dialog box.
b. Next add a vent.
X:0.8 m
Y:0.0 m
Z:0.5 m
X: 3.2 m
Y: 0.0 m
Z: 0.0 m
c. Next add an Opening:
X:0.8 m
Y:0.0 m
Z:1.0 m
X: 1.19 m
Y: 5.0 m
Z: 1.5 m
d. Next to add the adiabatic Floor:
X:3.0 m
Y:5.0 m
Z:0.0 m
X: 0.0 m
Y: 0.0 m
Z: 0.0 m
X:0.0 m
Y:5.0 m
Z:2.7 m
X: 0.0 m
Y: 0.0 m
Z: 0.0 m
Figure 2.10 The attributes of the wall at x=0
Figure 2.11 The screen picture after all the object were created
To activate the physical models
a. The Main Menu panel
. The top page of the main menu, as shown in figure 2.12, will
appear on the screen. The menu date may differ from that shown. 
Figure 2.12 The Main Menu top page.
While this panel is on the screen, you may set the title for this simulation, click on the 'Title' dialogue box. Then type in a suitable title, for example 'My first flow simulation'.
FLAIR always solves pressure and velocities. The temperature is also solved as the default setting.
Figure 2.13 The 'Models' page of the Main Menu.
b. To activate LVEL turbulence model
Figure 2.14 Select LVEL on the "Turbulence Models" page of the Main Menu.
To set the grid numbers and solver parameters
- 19 cells in the X-direction
- 20 cells in the Y-direction
- 19 cells in the Z-direction
Figure 2.16 Geometry menu page
This mesh is adequate for the example, but would need to be refined for a more accurate solution. The function of the Grid Mesh Settings dialog is explained in TR326.
Set the number of sweeps in this window to 500 as shown in figure 2.17.
Figure 2.17 Set the " Total number of iterations' to 300
Figure 2.18 Monitoring position
It can also be set by clicking on 'Output' on the main menu. For this case, the monitor-cell location, (11,19,7) will be displayed.
FLAIR uses the PHOENICS solver called 'Earth'.
To run Earth, click on 'Run', and then 'Solver', followed by clicking 'OK' to confirm running Earth. These actions should result in the PHOENICS Earth screen appearing.
As the Earth solver starts and the flow calculations commence, two graphs should appear on the screen. The left-hand graph shows the variation of pressure, velocity and temperature at the monitoring point that was set during the model definition. The right-hand graph shows the variation of errors as the solution progresses.
As a converged solution is approached, the values of the variables in the left-hand graph should become constant. With each successive sweep number, the values of the errors shown in the right-hand window should decrease steadily.
Figure 2.19 shows the EARTH monitoring screen at the end of the calculation.
Figure 2.19 The EARTH run screen at the end of calculation
Runs can be stopped at any point by following the procedure outlined below.
Please note: if the solver is stopped before the values of the variables in the left-hand graph of the convergence monitor approach a constant value, the solution may not be fully converged, and the resulting flow-field parameters may not be reliable.
2.3.4 Viewing the Results with VR-Viewer
The results of the flow-simulation can be viewed with the FLAIR VR post-processor called VR-Viewer.
In the VR-Viewer, the results of a flow simulation are displayed graphically. The post-processing capabilities of the VR-Viewer that will be used in this example are:
To access the VR Viewer, simply click on the 'Run' button, then on 'Post processor', then 'GUI Post processor (VR Viewer)' in the FLAIR-VR environment.
When the 'File names' dialog appears, click 'OK' to accept the current result files. The screen shown in figure 2.19 should appear.
Figure 2.19 The VR-Viewer screen picture as it appears for this case.
Viewing the Results with VR-Viewer
The detailed description of the VR-Viewer screen and hand set control buttons is provided in PHOENICS documentation TR326. This section simply gives instructions on how to view the results.
To view the results of the simple simulation just completed:
followed by the
'Vector toggle', 
. This will display velocity vectors on the current result plane (X plane).
You may use "Vector option" in the "Settings" menu to change the scale
factor for vectors. 
to set the
current results variable to temperature. Next, click on the 'Contour toggle', 
. Contours of
temperature are then displayed on the current result plane. 
to bring up the
Streamline management dialog box. Select 'Object' and 'Options', as shown in figure 2.20,
will bring up the 'Stream Options' dialog box shown in figure 2.21. 
Figure 2.20 The Streamline management dialog
Figure 2.21 Stream Options dialog box
Typical displays of a vector, contour and a streamlines plot are shown below in figures 2.22 (a - c) respectively.
Figure 2.22a Vector plot.
Figure 2.22b Contour plot.
Figure 2.22c Streamlines.
2.3.5 Printing from VR.
Screen images such as figures 2.22(a - c) can be sent directly to a printer by clicking on 'File', then on 'Print' from the main environment screen. A dialog similar to that shown in figure 2.23a opens.
Figure 2.23a Print Dialog Box
Alternatively, the screen image can be saved to a file by clicking on 'File', then on 'Save window as' from the main environment screen.
When 'Save window as' has been pressed, the dialog box shown in figure 2.23b opens.
Figure 2.23b 'Save Window as' Dialog Box
The 'Save as file' dialog offers a choice between GIF, PCX and BMP file formats, and allows the image to be saved with a higher (or lower) resolution than the screen image.
The graphics files are dumped in the selected folder (directory), with the given name. In all cases, the background colour of the saved image is that selected from 'Options', 'Background colour' from the VR-Editor main environment screen.
The above example has been designed to show how to use FLAIR to solve a very simple problem. More examples are provided in chapter 6, Tutorials, where how to use the different modeling objects, physical models and post-processing capabilities that are available in FLAIR are described in more detail.
3. The HVAC-specific object files and object types
3.1 The HVAC-specific object types
FLAIR provides six HVAC-specific object types, Diffuser, Fire, Jetfan, Spray-head, Person and People as described below.
The Diffuser is a single object representing a complex source of mass, momentum and energy. It is used to represent various types of diffusers found in rooms and buildings. The detailed implementation is based on the 'Momentum method' described in ASHRAE Report RP-100915.
The diffuser object can be accessed through the Object management dialog box. To load a diffuser object, click on the 'Obj' button on the main control panel to bring up the Object management dialog box. Then click on 'Object' , 'New' and 'New object' pull-down menu to bring up the Object specification dialog box. Select Diffuser from object 'Type' as shown in figure 3.1.
Figure 3.1 Selecting Diffuser from the object 'Type'
The default diffuser is the 4-way diffuser. Figure 3.2 shows the default diffuser attributes.
Figure 3.2 The default diffuser and its attributes
The following specifications can be defined through the attributes panel:
Diffuser type - there are 5 different types as shown in figure 3.3. Each type has its own shape.
Figure 3.3 The select diffuser type panel
The diffuser types have the following characteristics:
Figure 3.4 Round diffuser
Figure 3.5 Vortex diffuser, 45deg swirl angle.
Figure 3.6 4-way rectangular diffuser
Figure 3.7 4-way directional diffuser, all faces active
Figure 3.8 Grille diffuser, 45 deg symmetrical deflection
Figure 3.9 Displacement diffuser, 4 sides and top face active
Diffuser Attributes
All diffuser types can be rotated freely about any axis or combination of axes. Note however that if Grille, Round, Vortex or 4-way rectangular diffusers are rotated out of the plane of the grid, they must lie on the face of a BLOCKAGE object otherwise they will produce no flow.
Diffuser position - for all diffusers other than displacement, these set the coordinates of the centre of the mounting face of the diffuser. For displacement diffusers, it sets the low x,y,z corner.
Diffuser diameter - for round and vortex diffusers, this sets the diameter of the diffuser.
Diffuser size - for rectangular diffusers, sets the length of the faces.
Plane - This allows the user to place the diffuser in the X, Y or Z planes.
Side - When the diffuser is mounted internally in the solution domain, the diffuser itself can be on the decreasing-coordinate (low) or the increasing-coordinate (high ) side of the mounting face. The position boxes set the location of the mounting face - this controls whether the diffuser is above or below, to the left or right.
X/Y/Z Faces - For 4-way directional and displacement diffusers, these control which faces of the diffuser are active. The supply volume is divided uniformly amongst the active faces.
The face directions and deflection angles referred to below are always in the coordinate system of the diffuser itself, not taking into account any rotations. For example, consider a 4-way directional diffuser in the X-Y plane which has been rotated +90deg about Z. The high X face of the diffuser will now point along Y.
Supply pressure - This sets the pressure of the supply air, relative to the Reference Pressure set on the Properties panel of the Main menu (usually 1.01325E5 Pa). It is used together with the supply temperature to calculate the density of the supplied air. By default it is set to the ambient pressure, which is also set on the Properties panel. Any other value can be entered by switching to 'User'.
Supply temperature - This sets the temperature of the supply air in degree C. By default, it is set to the ambient temperature, which is set on the Properties panel of the Main menu. Any other value can be entered by switching to 'User'.
Supply volume - This sets the volumetric flow rate for the supply air in L/s or m3/s.
Set throw or effective area - The diffuser can be defined either in terms of the Effective area or Throw and terminal velocity. These factors are usually obtained from manufacturer's data sheets.
The Effective area can be deduced by dividing the supply volume flow rate by the discharge velocity. It is always less than the nominal plan area.
If the Throw and terminal Velocity are set, the discharge velocity and hence Effective area are deduced using a jet formula and the jet decay constant.
The depth of the diffuser (except grille and displacement) is deduced by dividing the Effective area by the active perimeter.
Swirl angle (for Vortex type only) - This sets the amount of swirl induced by the diffuser. A value of zero gives no swirl (equivalent to a round diffuser); the flow is purely radial. A value of 90 means the flow is purely tangential. Positive angles produce anti-clockwise swirl when looking down on the diffuser. This is usually the angle the diffuser blades are set to.
Angles from Z axis (for Grille/Nozzle type only) -
Figure 3.10 The Grille diffuser and its attributes
This specifies the deflection from the normal to the plane of the diffuser in each of the other two directions. If the plane is The default value of 0.0 means no deflection- the flow comes out normal to the diffuser surface. Positive values mean deflection in the + axis direction; negative values mean deflection in the - axis direction. The deflection is limited to +/- 89 degrees.
When the Symmetric Yes/No switch is set to Yes, the flow is divided symmetrically in the positive and negative axis directions. It is as if the grille were made up of two grilles with opposite deflection angles. When set to No, both halves use the same deflection angle. As the grille is divided horizontally and vertically, there are actually four sources for each grille.
Effective area ratio (for displacement type only) - For a displacement diffuser, this is the ratio between the true flow area and the modeled area. It is the same for all active faces.
The fire object is used to create an area or volumetric heat source, representing a fire. There are several options for setting the heat, mass and smoke sources at the fire. It is assumed that the mass released by the fire is the products of combustion, and that the SMOK variable represents the local mass fraction of combustion product.
Some combinations require the Heat of Combustion Hfu and the stoichiometric ratio, Rox to be set. If the product mass-fraction SMOK is solved, these values are set in Main menu - Solve smoke mass fraction - settings. If SMOK is not solved, these settings can be made on the Fire object dialog.
The fire can be loaded through the Object management in the same way as described in section 3.1.1 above for the diffuser.
The default fire object and its attributes are shown in figure 3.11 below.
Figure 3.11 The fire and its default attributes
The dialog will change as different options are selected, showing input boxes for the various parameters.
Heat Source
The heat source set here is the total heat source Qt =Qconvective + Qradiative. If the radiation model is not active, the heat source reported in the solution (as 'Source of TEM1') is reduced by the Radiative fraction Rf to be just the convective part. The Radiative factor is set on the 'Smoke settings' panel of the Main Menu, and is defaulted to 0.3333. The total heat release rate is still used to derive the smoke mass source
The options for the Heat source are:
Figure 3.12 Fire heat sources
Qt = mass*Heat of Combustion / (1+Rox)
If the Heat of Combustion is not constant, use 'From table file' for both the heat and mass sources.
Qt = a + b*(T+TEMP0)
where TEMP0 is the reference temperature.
If T is below Tmin or above Tmax, these values are used in the formula.
Qt = min(Qmax, a*(t-t0)b)
where Qmax is the maximum permitted heat release rate, t0 is the time at the start of the fire, and a and b are constants.
It has been found that the heat release rate grows approximately as the square of the time i.e. the b constant above is 2.0. Characteristic growth times and constants for various classes of fire are given in Table 10.1 of the CIBSE Guide E, Fire Engineering (Ref 4).
| Fire class | Characteristic growth time (s) |
Constant a (W/s2) |
| Ultra-fast | 75 | 187.6 |
| Fast | 150 | 46.9 |
| Medium | 300 | 11.7 |
| Slow | 600 | 2.9 |
Qt = Q(n-1) +(t-t(n-1)) / (t(n)-t(n-1))*(Q(n)-Q(n-1))
Time,Qt
0,0
60,350000
120,700000
180,1050000
240,1400000
300,1400000
360,1400000
420,1400000
480,1400000
540,1400000
600,2055000The Earth solver will perform a linear interpolation in the table to find the heat source for any particular time. The time in the table is the time since ignition. This option allows for any number of points in the table, and should be used in preference to 'Piece-wise Linear in time' if there are more than 10 points.
In a transient case, a file called 'heat_sources.csv' will be created. It will contain the convective heat source for each fire object for each time step. An example is given here:
Time , FIXMAS , POOL ,
PWLM , FIXT ,
FIXQ , LINTEM ,
3.000E+01, 1.100E+05, 7.705E+05, 1.719E+03, 0.000E+00, 1.320E+06, 1.005E+05,
9.000E+01, 1.100E+05, 1.346E+06, 5.156E+03, 2.747E+05, 1.320E+06, 1.005E+05,
1.500E+02, 1.100E+05, 2.011E+06, 8.594E+03, 2.747E+05, 1.320E+06, 1.005E+05,
2.100E+02, 1.100E+05, 2.753E+06, 1.203E+04, 2.747E+05, 1.320E+06, 1.005E+05,
2.700E+02, 1.100E+05, 3.561E+06, 1.547E+04, 5.493E+05, 1.320E+06, 1.005E+05,
The first column is the solver time, at the mid-point of each time step. The subsequent columns are the heat release rates in Watts for the FIRE objects named in the first row.
Mass Source
The options for the Mass source are:
Figure 3.13 Fire mass sources
The mass released is taken to be the products of combustion:
1kg Fuel + Rox kg Oxygen = (1+Rox) kg Product
Mass = Qt * (1+Rox) / Heat of Combustion
If the Heat of Combustion is not constant, use 'From table file' for both the heat and mass sources.
Area = a + b * tc
Mass = Area *( 1-exp(-B*Area.5))
Mass=M(n-1) +(t-t(n-1)) / (t(n)-t(n-1))*(M(n)-M(n-1))
Time, Mass
0, 0
60, 0.0073
120, 0.0219
180, 0.0365
240, 0.051
300, 0.0583
360, 0.0583
420, 0.0583
480, 0.0583
540, 0.0583
600, 0.072
The Earth solver will perform a linear interpolation in the table to find the mass source for any particular time. The time in the table is the time since ignition. This option allows for any number of points in the table, and should be used in preference to 'Piece-wise Linear in time' if there are more than 10 points.
In a transient case, a file called 'smoke_sources.csv' will be created. It will contain the product mass (smoke) source for each fire object for each time step. An example is given here:
Time , FIXMAS , POOL ,
PWLM , FIXT ,
FIXQ , LINTEM ,
3.000E+01, 2.000E-02, 1.401E-01, 3.125E-04, 8.182E-05, 2.400E-01, 1.828E-02
9.000E+01, 2.000E-02, 2.446E-01, 9.375E-04, 8.182E-05, 2.400E-01, 1.828E-02
1.500E+02, 2.000E-02, 3.656E-01, 1.562E-03, 8.182E-05, 2.400E-01, 1.828E-02
2.100E+02, 2.000E-02, 5.005E-01, 2.187E-03, 8.182E-05, 2.400E-01, 1.828E-02
2.700E+02, 2.000E-02, 6.474E-01, 2.812E-03, 8.182E-05, 2.400E-01, 1.828E-02
The first column is the solver time, at the mid-point of each time step. The subsequent columns are the mass release rates in kg/s for the FIRE objects named in the first row.
Scalar Source
The options for the Scalar source are:
Figure 3.14 Fire smoke sources
The SMOK scalar is taken to be product of combustion - the inlet value is therefore always 1.0. The parameters determining how the smoke concentration affect visibility are all set in Main menu - Solve smoke mass fraction - settings.
mass = Qt (1+ Rox)/ Heat of Combustion
This is then used to set the scalar source.
Note that some of the source types are only available for transient simulations. Not all source types are mutually compatible - for example if the mass source is 'heat related', the heat source cannot be 'mass related'. Such incompatible combinations will be flagged up as errors when trying to set them.
InForm - InForm sources are set through the InForm Commands button. This leads to a dialog from which a selection of InForm commands can be attached to this object. It is described here.
The jetfan object is used to create a volume of fixed velocity, representing the effects of a jetfan. The velocity components in the domain X-, Y- and Z-axes are calculated internally to give the set total velocity and direction.
The jetfan can be loaded through the Object management in the same way as described in section 3.1.1 above for the diffuser.
The default jetfan object and its attributes are shown in figure 3.15 below.
Figure 3.15 The jetfan and its default attributes
Fan type - The fan can be rectangular or circular in cross-section. Unless the grid is very fine, the difference will be mainly visual.
Xpos, Ypos, Zpos - Sets the location of the centre of the jetfan object. Any rotations set will be about this point.
Length - Sets the length of the jetfan in the X co-ordinate direction of the jetfan.
Width - Sets the width of a rectangular jetfan in the Y co-ordinate direction of the jetfan.
Depth - Sets the depth of a rectangular jetfan in the Z co-ordinate direction of the jetfan.
Diameter - Sets the diameter of a circular jetfan.
Velocity - Sets the delivery velocity of the jetfan in the X co-ordinate direction of the jetfan. The jetfan always blows along its own X-axis. The jetfan can be rotated about its centre to point in any desired direction.
Set turbulence intensity - when Yes, sets the turbulence intensity for the jetfan. Typical values may be in the range 20 - 25%. The turbulence quantities are set from:
KEjet = (Intensity/100 * Velocity)2 ; EPjet = 0.1643*KEjet3/2/(0.1*diameter)
For a rectangular jetfan, the diameter is taken as 0.5*(Height+Width).
When No, the jetfan has no direct impact on the turbulence field other than by creating additional velocity gradients.
The default setting is No. When switched to Yes, a value of 22% is set.
Heat load - Sets the heat gain (or loss) through the jetfan. The default setting of 0.0 ensures there is no heat gain or loss. Positive values represent a heat gain, as through a heater, negative values represent a loss, as through a cooler.
Angle to X axis - Sets the inclination of the jetfan X co-ordinate to the domain X-axis. The resulting flow direction is as shown in the table below:
| Angle | Jet direction |
| 0 | +X |
| 90 | +Y |
| 180 | -X |
| 270 | -Y |
Angle to Z axis - Sets the inclination of the jetfan X co-ordinate to the domain Z-axis. The default angle of 90 directs the jet parallel to the floor. Angles > 90 incline the jet towards the floor, angles < 90 incline the jet towards the ceiling.
The spray-head is the sprinkler designed for fire extinction. It works with the GENTRA module (see Encyclopaedia in POLIS). The spray-head can be loaded through the Object management in the same way as described in section 3.1.1 above for the diffuser.
The default spray-head object and its attributes are shown in figure 3.16 below.
Figure 3.16 The default spray-head object
The following specifications can be defined in the attributes dialog box:
Spray axis direction - This sets the axis of the spray to be along the positive X, Y or Z axis. The spray-head disk is normal to the selected axis.
Spray position - This sets the location of the centre of the spray-head disk. The disk is always normal to the spray axis.
Spray radius - This sets the radius of the spray-head disk. The droplet injection ports are uniformly distributed along the circumference of the disk.
Number of ports - This sets the number of the injection ports around the circumference of the spray disk.
Total volume flow rate - This sets the total volumetric flow rate of the water to be injected from the spray. The total amount is divided equally among the injection ports. The units are always litres/second.
Total injection velocity - This sets the velocity with which the droplets are deemed to be injected.
Spray angle (from spray axis) - This sets the angle between the spray and the spray axis. When set to 0.0, the droplets will be injected in the direction of the positive spray axis. Usually this will mean vertically upwards. When set to 90, the droplets will be injected normal to the axis. Usually this will mean horizontally. When sets to 180, the droplets will be injected in the direction of the negative spray axis. Usually this will mean vertically downwards.
Injection temperature - This sets the temperature of the injected droplets. The units are always degree C.
Volume median diameter - 50% of the water, by volume, is contained in droplets of this or greater diameter. Other 50% is contained in smaller droplets.
Number of size ranges - This sets number of droplet size to be considered. When sets to 1, the droplets will take volume median diameter. When sets to greater than 1, the sizes used will lie between the set minimum and maximum values, and will be distributed according to the Rosin-Ramler droplet distribution function.
Calculate link temperature (appears for transient run only) - This determines whether the link temperature for the spray will be calculated or not. If 'Calculate link temperature' is set to 'Yes', then two more entries, Activation temperature and Response time Index, will appear. The Track start- and end-times will be reset to 'Auto-on', and a new data entry box will appear for setting the duration of the spray after initiation.
Activation temperature is the temperature at which the track is to start.Response Time Index (RTI) is a measure of the detector sensitivity.
The link temperature is calculated from17:
dTl/dt = e(|Vel|) (Tg-Tl/) / RTIwhere Tl is the link temperature, Vel is the gas velocity and Tg is the gas temperature.
The calculated link temperatures are written to the file 'tlink1'csv' at the end of each time step. If there are more than 20 sprays, each group of 20 will be written to a separate 'tlinkn.csv' file where n is 1,2,3 etc.
A tutorial is provided in section 6.9 which shows how to use the Spray-head object for the simulation of fire extinction.
If GENTRA is not active at the time the first spray-head object is created, it will be automatically turned on, with all settings made for the spray model. Only the spray start- and end-times need be set for a transient case, should the spray not be active all the time.
If GENTRA is already turned on, it will be assumed that all settings as correct, and no default settings will be made.
The settings made for GENTRA are:
The Person object represents the heat load effect of a single human being. It does not apply a resistance to motion.
Figure 3.17 The default Person object
The 'Posture' button allows a choice of 'Standing' (as in the image above), 'Sitting' or 'User'. If 'User' is selected, the Size and Position dialogs on the Object Specification dialog can be used to size and rotate the image. The 'Facing' button toggles through +X,-X,+Y and -Y to determine which direction the person faces.
The heat source can be Total heat in W, of fixed temperature in Centigrade.
The People object is used to represent the heat load of a large number of people, for example the audience in a theatre. It does not apply a resistance to motion.
Figure 3.18 The default People object
The predefined HVAC-specific object files contain both geometry information and the default attributes of the object or assembly. They are stored in the directory /phoenics/d_satell/d_object/public/flair and its subdirectories as described below.
3.2.1 Cabinets subdirectory contains the following object files:
.
Figure 3.19 The casing assembly
A double click on each component brings up the object specification dialog, and then a click on 'Attributes' button brings up the panel showing that the material of all the thin-plates and the plates as shown in figure 3.20a and figure 3.20b respectively.
Figure 3.20a The default attributes of the thin-plate of the casing assembly
Figure 3.20b The default attributes of the plate of the casing assembly
The user can scale the casing assembly and place it in a desired location or modify the attributes of individual components.
It is also possible for the size and the location of individual component to be modified if the component is disconnected from the assembly.
Figure 3.21 The rackunit assembly
The default attributes of the individual inlets are shown in figure 3.22(a-c) respectively.
Figure 3.22a The default attributes of an inlet of the rackunit assembly
Figure 3.22b The default attributes of an inlet of the rackunit assembly
Figure 3.22c The default attributes of an inlet of the rackunit assembly
3.2.2 Jetfans subdirectory contains the following model files:
Figure 3.23 The Fan+x20 assembly
The internal fan is located in the middle of the duct and its attributes are shown in figure 3.24.
Figure 3.24 The attributes of the fan
3.2.3 Living subdirectory contains the following model files
Figure 3.25 The sitting-man and the standing-man
Figure 3.26 The attributes of the sitting-man
3.2.4 Perforated Plates subdirectory contains
Figure 3.27 The default attributes of the perforated plate
3.3 How to import the HVAC objects
Figure 3.28 The Object Management dialog box
Figure 3.29 The Import Object dialog box
All the object files (.pob file) are kept in the directory d_object/public/flair and its subdirectories. The supplied objects are divided into a number of classes, with fairly self-explanatory names, for example, a casing can be found in flair/cabinets directory.
Figure 3.30 The default position of the selected object
Figure 3.31 The object specification dialog box
For a single object, simply click on the 'Attributes' button on the 'General' dialog box, and an object attributes dialog box will appear on the screen. For an assembly object, the user needs to click on 'Name' to select a component of the assembly object; and the user can examine or modify the default attributes as shown in figure 3.32 for the component B4 of the casing assembly.
Figure 3.32 The object attributes dialog box
Clicking on the 'Export' button brings up the dialog box shown in figure 3.33, which is used to export an object file. The user has the options to save the attributes or the geometry data or both. The user has the 'browser' to find the directory where he puts the object file, otherwise the object file will be in your working directory.
Figure 3.33 The object export dialog box
The 'Size' button is used to check the size of the imported object and then scale or re-size it.
The 'Place' button is used to see the position of the imported object and re-position or rotate it about its own axis.
The 'Option' button is used to change the colour of the imported object and to choose the rotation centre and rotation mode.
The 'Shape' button is used to import custom shapes as follows.
The detailed operations about how to import custom geometry can be found in PHOENICS documentation Tr326.
As a special version of PHOENICS, FLAIR has the following HVAC-related models: system curve, fan operating point, humidity calculation, comfort index and smoke movement.
This chapter is to provide detailed descriptions about how to activate these models.
All these models can be set up through the Main Menu in FLAIR VR-Editor. The main menu
is reached by clicking the Main Menu button, 
on the hand-set.
This brings up the Main Menu top panel.
Figure 4.1 is the top panel of the main menu, and can be reached from any other panel by clicking on Top menu. It is the panel displayed whenever the Main menu is activated from the hand-set of the FLAIR VR-Editor.
Figure 4.1 Main menu top panel
The buttons along the top of the panel allow the setting and modification of the case. Some of those buttons have been used for the simple example described in section 2.3 above and more buttons will be used in Chapter 6, Tutorials, a complete description of functions for each button can be found in PHOENICS documentation TR326. This section only describes the "Models" button.
During the design stage, it may be useful to know the system characteristic in order to be able to choose the appropriate Fan for the equipment.
Click on "Models" button will bring up the panel shown in figure 4.2.
Figure 4.2 The "Model" panel
If you set the System curve button to ON, "Settings" button will appear. The "Settings" dialog box is shown in figure 4.3 which enables you to perform simulation of the flow through your system, using different flow-rates and obtaining several pairs of data (flow-rate vs. pressure drop) allowing you to plot the system curve.
Figure 4.3 The System curve dialog box
The 'Settings' allow the user to specify:
The user may also find extracted data and a line-printer plot of the curve in their result file.
Note that Fan-setting cannot be active at the same time as system-curve calculation; therefore, if when the user activates system-curve Fan-setting is active, it will automatically become de-activated.
Although the user can specify a constant total mass flow rate in FLAIR, in real world applications, the performance of a fan is described by its characteristic curve.
The relationship between volumetric flow rate and the pressure drop across the fan (static pressure) is described by the fan characteristic curve, which is usually supplied by the fan manufacturer as shown in figure 4.4. The total volumetric flow rate, is plotted against fan static pressure.
Figure 4.4 An example of the Fan flow characteristics
If your requirement is to choose the fan which will be appropriate for the equipment you are designing, you may need to perform 'system curve' simulation (see section 4.1.1) in order to obtain the 'system characteristics' which would then be used to determine the fan 'operating point' which occurs at the intersection of the system curve with the fan characteristic curve.
The 'Fan operating point' option in 'Models' menu in FLAIR automates this procedure; you are only required to specify the fan characteristic curve in tabulated form, and FLAIR will calculate the 'operation point'.
When the "Fan operating point" option is activated, FLAIR will compute the fan operating point for a given fan characteristic curve using an iterative method as follows:
This option works in the same manner for a single fan and for multiple fans each having different characteristic curve.
Fans in parallel are treated as separate fans with the combined characteristics of each fan. Fans in series are treated as a single fan with the combined characteristics.
At the end of the result file, you will find information about the operating point of your fan-system combination.
Note that fan-setting cannot be active at the same time as system-curve calculation; therefore when you activate fan-setting, if system-curve is active it will be automatically de-activated. At least one FAN object must exist before this option can be activated.
How FLAIR stores the fan flow characteristic curve
The fan flow characteristic curve is stored in a file called 'FANDATA'. The file can contain information for up to 50 fans. The format for each fan is:
Fan title (up to 16 characters).
Number of data pairs for the fan (single integer up to 100).
Two columns of numbers: first column is flow-rate in m^3/h; and second column is pressure-drop in Pa.
Example of Fan data
FAN1 5 0. 8. 30. 6. 60. 4. 90. 2. 120. 0.
It shall reside in the current working directory.
When 'Fan operating point' is active, a 'Settings' button appears, which leads to this page:
Figure 4.5 The Fan Operating Point Settings panel.
To use the "Fan Operating point" option, you need to do the following:
In section 7.6, there is a tutorial example which provides step-by-step instructions on how to activate the "Fan Operating Point" option for a single fan mounted at a boundary of a cabinet.
FLAIR provides for five comfort index calculations:
Clicking on the Comfort Index button leads to a panel where any or all of the three calculations can be activated, and relevant input parameters set.
Thermal comfort index, or dry resultant temperature, is a standard index used to show the level of comfort within the occupied space. It is a function of air temperature, air velocity and mean radiant temperature. The formula as defined in Volume A of the CIBSE Guide is:
Tres = ( Trad + Tair * (10*vel) 0.5) /( 1+ (10* vel) 0.5)
Where Tres is the resultant temperature; Trad mean radiant temperature; Tair air temperature; vel air velocity.
The mean radiant temperature can be a user-set constant value, or can be taken to be the T3 radiation temperature of the IMMERSOL radiation model as shown in figure 4.6.
Figure 4.6 The Comfort index dialog box
Comfortable values of Tres are typically in the range 16-28 deg C, depending on the external conditions and type of occupancy.
PMV is an index defined in ISO 7730 that predicts the mean value of the votes of a large group of people on a 7-point thermal sensation scale:
+ 3 hot
+2 warm
+1 slightly warm
0 neutral
-1 slightly cool
-2 cool
-3 cold
Figure 4.7 PMV dialog box
For the PMV option, the following input parameters are required:
The radiant temperature - this can be a user-set constant value, or can be taken to be the T3 radiation temperature of the IMMERSOL radiation model.
The clothing insulation - clothing insulation is measured in
'clo' (clothing unit)
'tog' (European unit of thermal insulation) or
m2 k/w
where
1 clo = 0.155 m2 k/w
1 tog = 0.645 clo
The practical range is between 0 clo (no clothing) and 4 clo (Eskimo clothing); 1lb (0.454kg) corresponds roughly to 0.15 clo, with 0.6 clo and 1.0 clo being typical of summer and winter clothing respectively.
The default value is 0.6 clo.
The Metabolic Rate - is measured in 'met' (metabolic units) or W/m2; 1 met = 58.15 W/m2. The appropriate value depends on the activity being undertaken (see ISO 7730 and ISO 8996):
0.8 met - reclining
1.0 met - seated, relaxed
1.2 met - sedentary activity (office, dwelling, school, laboratory)
1.6 met - standing, light activity (shopping, laboratory, light industry)
2.0 met - standing, medium activity (shop assistant, domestic work, machine work)
1.9 met - walking on the level at 2 km/h
2.4 met - walking on the level at 3 km/h
2.8 met - walking on the level at 4 km/h
3.4 met - walking on the level at 5 km/h
The default value is 1.2 met.
The external work - is the part of the metabolic rate that is used up in the activity being performed, rather than contributing to the heat balance of the individual concerned. It is usually taken as zero, and should always be less than the metabolic rate.
The default value is 0.0.
The relative humidity - individual comfort is influenced by the humidity of the air, which affect the heat loss through the skin. It is often sufficient to specify a reasonable value for a particular environment, but it is also possible to calculate the humidity as part of the simulation.
If humidity is calculated it is important to specify realistic conditions at domain inlets and at sources (people, surfaces).
The default value is 50%.
PPD is an index defined in ISO 7730 that predicts the percentage of a large group of people who are likely to feel too warm or too cool, i.e the percentage of a large group of people who would vote for values other than 0, -1 or +1 on the thermal sensation scale used for PMV.
The required input parameters are the same as for PMV.
PPDR is defined in ISO 7730 as the percentage of people dissatisfied due to draught, using the following equation:
PPDR = (34-Ta)*(V-0.05)0.62*(0.37*V*I+3.14)
where Ta is the local air temperature, V is the local air velocity and I is the local turbulence intensity in %. In Flair, it is derived from the local turbulence quantities and the local absolute velocity.
I = 100*k0.5/V
where k is the local turbulent kinetic energy (KE).
PLOS, the loss in performance in % by people occupying the space, is defined by Roelofsen3 as:
PLOS = b0 + b1PMV + b2PMV2 + b3PMV3 + b4PMV4 +b5PMV5 + b6PMV6
where PMV is the local Predicted Mean Vote and the regression coefficients b1 - b6 are given in the table below:
| Regression coefficient |
Cold side of comfort zone |
Warm side of comfort zone |
| b0 | 1.2802070 | -0.15397397 |
| b1 | 15.995451 | 3.8820297 |
| b2 | 31.507402 | 25.176447 |
| b3 | 11.754937 | -26.641366 |
| b4 | 1.4737526 | 13.110120 |
| b5 | 0.0 | -3.1296854 |
| b6 | 0.0 | 0.29260920 |
This quantity represents the time since entry at each point in the domain. The units are seconds.
In 'dead' zones, such as in recirculation areas, the time since entry will tend to a large value as the air will be trapped there. These values should be treated as indicative rather than exact. In regions where there is a reasonable exchange of air, the values will be correct.
The variable name for plotting in the Viewer is AGE.
If the 'Solve Specific humidity' button is switched to 'On'. the specific humidity equation, MH2O, will be solved. The variable, MH2O has units of kg water vapour/kg mixture. It is a mass fraction of water vapour.
By clicking on 'settings', the dialog box shown in figure 4.8 will appear.
Figure 4.8 Humidity Ratio and Relative humidity can be derived
Several derived quantities can be displayed. These are:
Humidity ratio, which has units of (g/kg)
If the Humidity ratio button is set on On, the humidity ratio in g/kg will be derived. The variable name for plotting in the Viewer is HRAT.
Relative humidity (%)
If the Relative humidity button is set to On, the relative humidity in % will be derived. In this case, the water-vapour saturation pressure, partial pressure and mole fraction are also made available for storage as shown in figure 4.9.
Figure 4.9 Relative humidity dialog box
The variable name for plotting in the Viewer is RELH.
As seen from figure 4.9, if the relative humidity is activated, the following quantities which are used in the derivation of relative humidity can also be stored:
The units used to specify boundary sources (inlets, openings, volume sources) can be set on the dialogs for the individual objects.
The options are:
The default is Specific Humidity
If the 'Solve smoke mass fraction' button is switched to 'ON', FLAIR will solve an equation for the mass-fraction of a passive contaminant, usually the products of combustion from a fire.
If the solve smoke mass fraction button is set to ON, the parameters controlling the smoke production by the fire can be set from the 'settings' menu as shown in figure 4.10.
Figure 4.10 Smoke production parameters
The parameters are:
The default values were derived from experiments on the burning of a car vehicle using a Heat Release Rate (Qt) of 6MW, and a Heat of Combustion (Hfu) of 25 MJ/kg.
The total heat release rate Qt, mass consumption rate of fuel Mf and heat of combustion Hfu are linked by:
Qt = h * Mf * Hfu
where h is the combustion efficiency. The Heat of Combustion to be entered is an effective Heat of Combustion, in that it already includes h.
The mass generation rate of product is then derived from
Mp = (1+Rox) * Mf
For example, when the fire mass source is set to 'Heat related', the following expression is used:
Mp = Qt * (1+Rox) / Hfu
If the radiation model is not used, the heat release to the fluid domain should be reduced by the radiative fraction Rf (the portion of heat which is transferred directly by radiation). The CIBSE Guide E [20034] indicates that (1-Rf) is of the order 1/1.5 (=0.6667) i.e. Rf=0.33333.
The heat release set for the FIRE object is the total heat, Qt. This is used to deduce the smoke mass source, but is multiplied by(1-Rf) for use as the convective heat source. Strictly speaking, the radiative part of the heat release should be spread over the surrounding surfaces, but this is rarely done in practice.
If the radiation model is used, Rf is set to 0.0, as the partitioning between radiative and convective transfer is being modeled.
4.6.1 Optical smoke density
The smoke resulting from a fire is associated with reduced visibility owing to the light scattering and absorption properties of the soot particles. Therefore, only a certain fraction of light can pass through the smoke, and the optical density of smoke provides a measure of the light obscuration properties of the solid particles. The fraction of light passing through a smoke layer of a given thickness L is given by the Beer-Lambert law [Tuomisaari, 199716], which can be expressed as:
I/Io = 10(-DL) (1)
where I is the intensity of light in the presence of smoke, Io is the intensity in the absence of smoke, L is the optical path length, and D is the optical density with units of m-1. The above equation can also be expressed in terms of natural logarithms [Tuomisaari, 199716], so that:
I/Io = e(-KmCs,pL) (2)
where Km is the mass specific extinction coefficient of the smoke aerosol in m2/kg, and Cs,p is the mass concentration of the smoke aerosol in kg/m3:
PHOENICS-FLAIR solves for the mass-fraction variable SMOK, which represents the mass fraction of smoke as products of combustion Cs in kg-smoke/kg. The mass concentration of particulate smoke Cs,p is computed from:
Cs,p = r Ys Cs /(1+Rox) (3)
where r is the mixture density, Ys is the particulate smoke yield in kg-smoke/kg-fuel, and Rox is the stoichiometric coefficient in kg-oxygen/kg-fuel. The value of Rox can be derived by assuming that
Hfu= b Rox (4)
where Hfu is the heat of combustion of the fuel (J/kg), and b is an empirical constant reported to be within ±5% of 13.1MJ/kg-fuel for most common combustible species (Babrauskas et al [198513, 199211,12] ). From equations (1) to (3), it follows that the smoke optical density is given by:
D = Km Cs,p/2.3 = Km r Ys Cs /(2.3 (1+Rox)) (5)
In the literature, it has been established empirically that the value of Km can be considered as a constant the order of 7000 to 8000 m2/kg [4,7,8]. For example, these references suggest the value of 7600 m2/kg for the flaming combustion of both wood and plastics.
The optical density is made available for plotting in the Viewer as the variable OPTD.
4.6.2 Visibility - Sight length or Visibility distance
The visibility in smoke is defined as the furthest distance d at which an object can be perceived, and it is computed from [4,5]:
d = A / Km Cs,p (6)
where A is an empirical coefficient with A=3 for light-reflecting signs, and A=8 for light-emitting signs [4,5]. Light emitting objects such as electric lights or illuminated signs are more easily perceived than light-reflecting objects which receive ambient illumination.
The relationship between visibility distance and optical smoke density can be deduced from equations (5) and (6) as:
d = 2.3 A/D (7)
The CIBSE fire-engineering guide [4] suggests that people are reluctant to proceed through smoke if the visibility is less than 8m, and so for the purposes of escape, the visibility should be at least this value.
In PHOENICS-FLAIR the sight length (or visibility) is calculated according to:
SLEN = min(Dmax, d)
The visibility coefficient Dmax is defaulted to 30.0m, and this simply ensures that the sight-length has a finite rather than infinite value in smoke-free regions.
Two sight length variables are provided, SLEN which has A defaulted to 3.0, and SLN2 which has A defaulted to 8.0.
In earlier versions of Flair (pre 2008), the sight length was defined as:
SLEN = min(C, A'/(B*r*SMOK))
The default values employed by PHOENICS for the visibility coefficients A' and B were related to car fires in parking garages with sufficient supply of air. The smoke production & potential in an air-poor environment ( a car in a small garage or several cars burning together) will be significantly higher.
The coefficient B which took the value of 137 was computed from a smoke potential SP of 400m2/kg and a stoichiometric ratio Rox of 1.923 kg oxygen per kg of fuel (B=SP/(1+Rox)). The values of SP and Rox were derived from experiments on the burning of a car vehicle using a Heat Release Rate (Q) of 6MW, and a Heat of Combustion (H) of 25 MJ/kg. A' was 1 for light-reflecting objects and 2.5 for light-emitting objects.
Comparing the sight length formulae, we see that
Ys = A * B * (1+Rox)/(A' * Km)
Taking A=3; B=137, Rox=1.923, A'=1.0 and Km=7600, we get Ys=0.158
Further smoke-potential values can be found in the literature (see for example Drysdale [20009] and Hushed [200410]).
The visibility coefficient C is now Dmax.
4.6.3 Light Intensity Reduction
An alternative to sight length is to calculate the reduction in light intensity due to the smoke. The Beer-Lambert Law can be used to deduce the effect of the smoke on light intensity
LR = 100.* Iz / Io
= 100.*e ( - S ( Cs*r*Km * dz) )
where dz is the distance along the path from a point to the point being looked at. Iz is the light intensity at the current point, and Io is the intensity at the origin. LR is then the percentage reduction in light intensity. When the light intensity is reduced to less than 0.16% of the original, the object is no longer visible.
In Flair, this has been implemented as a post-processing option in the Viewer. Starting at the probe, an integration is carried out along straight lines between the probe and each cell centre. A variant of the particle tracking routine is used for this purpose. Whenever a solid cell or blocked face is encountered, the integration is stopped and the intensity ratio is set to 0.0, as the probe cannot be seen from further along that path.
For a fine grid, the calculation can be quite lengthy as in principle the number of integrations is NX*NY*NZ-1. If some areas can be guaranteed not to be visible e.g. other floors, some time can be saved by restricting the plotting range to exclude the unwanted areas. To do this, go to the 'Plot Limits' tab of the Viewer Options dialog and set the volume for plotting (and integrating).
The steps in activating and displaying the light reduction ratio are:
- Place the probe at the point to be looked at. This will often be the middle of the fire object.
- Click the Main Menu icon
icon on the Tool Bar to bring up the Viewer's Domain Dialog
- Click 'Go' to calculate the distribution of light intensity reduction.
- A new variable called 'Light Ratio' is created and added to the end of the list of variables available for plotting.
- The light intensity ratio can be displayed as contour maps or iso-surfaces of the Light Ratio variable.
In the above image, the fire is not visible from anywhere to the right of the iso-surface, either because the view is blocked by the plate object, or because it is obscured by the smoke.
- In transient mode, the light ratio will be re-calculated (based on the current probe position) each time the time step is changed (by pressing F6, F7, F8 or
), provided that the current plotting variable is 'Light Ratio'. For large grids there may be a noticeable delay between time steps as the integrations are performed.
4.6.4 Derived quantities
In addition to the solved-for combustion-products mass fraction (SMOK), the two sight length variables SLEN and SLN2 and the optical density OPTD, the following derived quantities can be calculated and stored:
- Product density (kg/m^3) (SDEN) = r * SMOK
- Product concentration in parts-per-million (PPM) = 106 * SMOK
- Particulate concentration in parts per million (PPPM) = 106 * Ys *SMOK / (1+Rox)
- CO concentration in parts per million (COPM) = 106 * Yco * SMOK / (1+Rox)
where Yco is the CO yield in kg-CO/kg-fuel.
4.6.5 Fire products data
For various fire materials, Table 4.6.3.1 provides suggested values of heats of combustion and yields of smoke particulates and carbon monoxide ( see CIBSE Guide E [20034] )
Material Hfu (MJ/kg) Yco (kg/kg) Ys (kg/kg) Timber 13.0 0.020 <0.01 - 0.025 PVC- Polyvinyl chloride 5.7 0.063 0.12 - 0.17 PU- Polyurethane (flexible) 19.0 0.042 <0.01 - 0.23 PU- Polyurethane (rigid) 17.9 0.18 0.09 - 0.11 PS- Polystyrene 27.0 0.060 0.15 - 0.17 PP- Polypropylene 38.6 0.050 0.016 - 0.1 Table 4.6.3.1 Fire data for flaming combustion
Heat release rates, heats of combustion and yields for other materials can be found in the literature. For example, Babrauskas et al [198513, 199211,12] examined the fire behaviour of upholstered furniture, and found that the data reported varied considerably with the component materials for the frame, cushioning material and upholstery fabric. Typical values for a traditional upholstered easy chair are Hfu=18MJ/kg, Yco=0.05kg/kg and Ys=0.025kg/kg. NFPA 92B [20056] lists heats of combustion and heat release rates for a large number of combustible materials.
The stoichiometric ratio Rox can be estimated from the heat release rate Q by assuming that the heat released per unit mass of oxygen is constant ( Huggett [198014] ). In the literature, this ratio Hfu/Rox is taken as 13.1 MJ/kg and varies by only ±5% for almost any common combustibles ( Babrauskas et al [198513, 199211,12] )
1. CIBSE Guide, Volume A, Design Data
2. ISO 7730 Second Edition 1994-12-15
Moderate thermal environments - Determination of the PMV and PPD indices and specification
of the conditions for thermal comfort.
3. Roelofsen, Paul. Journal of Facilities Management Volume 1, Number 3
November 2002 ISSN 1472-5967
The impact of office environments on employee performance: The design of the workplace as
a strategy for productivity enhancement
4. Fire Engineering CIBSE Guide E, ISBN 1 903287 31 6, CIBSE, London, (2003).
5. T.Jin, 'Visibility through fire and smoke', J.Fire & Flammability, Vol.9, pp135-155, (1978).
6. NFPA 92B, 'Standard for smoke management systems in malls, atria and large spaces', NFPA, Quincy, Massachusetts 02269-9101, USA, (2005).
7. G.W.Mulholland & C.Croarkin, 'Specific extinction coefficient of flame generated smoke', Fire & Materials, Vol.24, No.5, p227, (2000).
8. G.W.Mulholland, 'Smoke production and properties', Chapter 2, Section 13, p2-258, SFPE Handbook of Fire Protection Engineering, 3rd Edition, NFPA, Quincy, Massachusetts 02269-9101, (2002).
9. D.Drysdale, "An Introduction to Fire Dynamics", John Wiley, (2000);
10. B.P.Hushed, "Optical source units and smoke potential of different products" DIFT report 2004:1, DIFT, Denmark, (2004).
11. Babrauskas, V. "Generation of CO in Bench-Scale Fire Tests and the Prediction for Real-Scale Fires", Fire & Materials Int. Conf., Arlington, VA, USA, p155, (1992).
12. Babrauskas, V., J.R.Lawson, W.D.Walton & W.H.Twilley, "Upholstered furniture heat release rates measured with a furniture calorimeter", NBSIR 82-2604, USA (1992).
13. Babrauskas, V. & Krasny, J., "Fire Behaviour of Upholstered Furniture", NBS Monograph 173, NBS, USA(1985).
14. C.Huggett, 'Estimation of rate of heat release by means of oxygen consumption measurements', Fire & Materials, 4, 61-5, (1980).
15. Srebric, J., Chen Q., "Simplified Diffuser Boudary Conditions for Numerical Room Airflow Analysis", ASHRAE RP-1009, March 20, 2001
16. M.Tuomisaari, "Visibility of exit signs and low-location lighting in smoky conditions", VTT Publications 300, TRC of Finland, Espoo, (1997).
17. G.Heskestad & R.G. Bill, "Quantification of Thermal Responsiveness of Automatic Sprinklers Including Conduction Effects", Fire Safety Journal, 14:113-125, 1988.
In addition to the simple example described in chapter 2, this chapter provides further 9 examples, each of which gives step-by-step instructions, combined with pictures, show how to use various features in FLAIR to set up models, to run the solver and to view the result. These cases are:
Tutorial 1 Investigating library case I203 illustrates how to load a case from the FLAIR library, to investigate the model settings, to run the case and to view the results.
Tutorial 2 A room with two radiators shows how to activate the IMMERSOL radiation model. The 'Duplicate object' function is used for the creation of the second window and radiator. The material of the radiators is selected from the property data base. A fixed heat flux is used as the heat source for the radiators.
Tutorial 3 Comfort indices in a room is similar to tutorial 2, but adds a chair and a sitting person into the room. This tutorial demonstrates how to activate the comfort index option.
Tutorial 4 Fire in a room shows how to use the Fire object for simulating a fire in a room. Smoke movement is also simulated.
Tutorial 5 A room with sunlight describes how to use Shapemaker to create a sunlight object in the model building.
Tutorial 6 A cabinet with a fan illustrates how to use the 'fan working point' option and how to create a fan-data file for the simulation.
Tutorial 7 Flow in a computer room shows how to use 'Group' and 'Arraying objects' features to add the desks and computers. The case also shows how to load a round diffuser from the predefined HVAC object library.
Tutorial 8 Flow over Big Ben demonstrates how to import a CAD file in STL format into the FLAIR VR-Editor to create the geometry. This tutorial also shows how to use a Wind_profile object to describe the wind profile at the upstream boundary. The 'Paint' object capability in the VR-Viewer is used to draw the pressure contours on the object surface.
Tutorial 9 Fire-spray in a compartment shows how to use the spray-head object and GENTRA module for the simulation of a fire-spray in a compartment. This kind of application of the sprinkler is commonly adopted in a car park for fire extinction.
Tutorial 10 Fire modeling gives an example of the FIRE object for a typical t2 fire in a simple configuration. It also shows how the operation of jetfans can be controlled by a temperature sensor using InForm.
7. Q1 Settings
7.1 Diffuser
7.2 Fire
7.3 Jetfan
7.4 Sprayhead
7.5 Person
7.6 People
