Encyclopaedia Index

Flair User Guide

CHAM Technical Report TR 313

last revised 15.08.16

Contents

  1. Introduction
    1.1 What is FLAIR ?
    1.2 What FLAIR can assist its users to do
    1.3 What FLAIR users must do for themselves
  2. Getting started
    2.1 Modes of FLAIR operation
    2.2 Accessing the FLAIR on-line help
    2.3 A simple example
  3. The HVAC-specific object files and object types
    3.1 The HVAC specific object types
    3.2 The HVAC-specific objects and their default attributes
    3.3 How to import the HVAC objects
  4. HVAC-Related Models
    4.1 Main Menu - Top Panel
    4.2 System curve
    4.3 Fan operating point
    4.4 Solve pollutants
    4.5 Solve smoke mass fraction
    4.6 Solve specific humidity
    4.7 Comfort Index
    4.8 Mean age of air (AGE)
    4.9 Radiation Modelling
  5. References
  6. Tutorials
  7. Q1 Settings
    7.1 Diffuser
    7.2 Fire
    7.3 Jetfan
    7.4 Sprayhead
    7.5 Person
    7.6 People
    7.7 Pollutants
    7.8 Radiation

1. Introduction


1.1 What is FLAIR ?

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 computed temperature distribution in Hackney Town 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. But the following warning should be heeded.

A warning

One piece of CFD knowledge which users of FLAIR should possess is that CFD-based predictions always differ from the realities which they seek to simulate to some extent, for reasons which include: Users of FLAIR should therefore never suppose that what is predicted is therefore true. 'Is it plausible?' must always be asked; and, if practical experience evokes doubts, one of at least the above error sources should be searched for.

1.2 What FLAIR can assist its user to users to do

Many of the functions that are required to create a FLAIR model, to solve the problem, to examine the results and to activate on-line help, can be accessed through the single integrated FLAIR-VR interface.

1.3 What FLAIR users must do for themselves

Many of the required functions, yes; but not all. FLAIR can provide often-helpful default settings. But it cannot know what it has not been told; and its users must accept responsibility for the deciding what it should be told.

Physical input data

In the real world, floors are seldom smooth. In car parks they are usually of rough concrete, perhaps with raised ridges separating bays; in dwelling houses they may be carpeted; and grass or other vegetation is to be found out of doors. Only the user knows which is to be found, and where, in the scenario which it is hoped that FLAIR will realistically simulate.

FLAIR allows 'wall roughness' to be specified; but the user must estimate the magnitudes of the roughness lengths which are appropriate to the various surfaces.

In the majority of practical circumstances, solid objects and partitions are present which have thicknesses or surface irregularities which have too fine a geometrical scale to be realistically represented by the computational grid which covers the whole domain. It is the user who must decide whether FLAIR should ignore their existence; and, if not, which of its available devices should be activated to take approximate account of it.

For example, a metro-station platform may be crowded with people. The heat which they generate may be estimated and introduced to FLAIR as a volumetric heat source; and the space which they occupy by way of a volume porosity. But the effect of their presence on the flow of air is nor fully represented thereby; they exert resistances to the horizontal velocity components which require volumetric friction coefficients to be supplied also.

Similarly, car parks (by definition!) contain cars; and they certainly both provide a not-to-be-ignored resistance to the flow of air; and the eddies created between them augment the effective turbulent diffusion coefficients which FLAIR employs when calculating the distributions of temperature and pollutant concentration. That the FLAIR-VR interface happens to offer no specific means of representing these effects is no reason for ignoring them.

PHOENICS, the 'CFD engine' which underlies FLAIR, can represent the above phenomena by way of its In-Form (i.e. input-via-formulae) facility; but what formulae to employ? That the user must decide.

The decision is never easy to make; and for two reasons, namely:

Considerations such as these lead the to the most important thing which users must do for themselves, namely estimate the margin of error, bearing in mind:

What margin they decide to adopt is itself a matter of guesswork, must differ from scenario to scenario, and will vary from one aspect of a scenario to another. Rarely however will the reasonably cautious user feel confident in claiming limits closer than +/- 30%. Sometimes the range 10% to 1000% (for an essentially positive quantity) is more wisely accepted; and this is true not of FLAIR alone but of all predictive software based upon Computational Fluid Dynamics.


Numerical input data

The just-mentioned choice of grid fineness has a big influence. Words to be found in tutorials such as "the grid will be generated automatically", may cause readers to suppose that PHOENICS will generate the optimum grid. But a moment's thought shows that to be impossible; for 'optimum' implies balance of advantages; and PHOENICS cannot know the relative importances which the user would assign to numerical precision, physical realism and economy of computer time.

PHOENICS will by default create a grid which does not completely over-look the presence of any of the distinct objects which the user has referred to; but often this produces a worst-of-both-worlds grid: too fine for economy and too coarse for accuracy.

The following image illustrates such a situation. The user wished to calculate the spread of smoke from a burning car in car park.

He allowed PHOENICS to choose a grid which was fine enough to recognise the presence of the car, but far too coarse to represent realistically the flow around it. Moreover the grid is diagonally oriented relative to the wind direction and thus gives maximum inaccuracy in the spreading rate, caused by 'numerical diffusion'.

A better-instructed user would have:

His predictions would have been both more reliable and less expensively obtained.

Output

Each run of FLAIR produces an alphanumeric RESULT file; and a few items likely to be of interest to HVAC users are supplied together with those which result from perhaps-unchanged PHOENICS-default settings. But the latter are many and the former few; so the user may miss what is intended for him.

PHOENICS possesses however a simply activated mechanism for printing the few items which the user selects into a single file (called INFOROUT); and this enables him to see precisely what he wants to see, and (for the moment) no more.

PHOENICS, and therefore FLAIR also, offers several graphical-display modules to its user. VR-Viewer, PHOTON and Win-PHOTON are among them; and it offers tutorial which teach users how utilise them. Less prominently described however is the means of not controlling them oneself (which requires skill, and is time-consuming); but instead causing their images to be created automatically by way of macros, i.e. commands written into a file which, when it receives it, the display package understands. All the PHOENICS packages can be operated in this manner.

The FLAIR user is therefore advised that, if he wishes, he can do much more for himself than FLAIR does automatically for him. He can find out about these from CHAM's User Support, from a more knowledgeable-than-he friend, or from the PHOENICS On-Line Information System, POLIS, accessible here or here.

Assessing plausibility

Every user makes mistakes at some time when inputting data, for example giving the gravitational acceleration a positive instead of a negative sign; or using kilojoules per second rather than watts for heat fluxes. The first may cause fluid to rise rather than sink; and the latter may cause generate physically improbable temperatures. But these implausible effects may escape the attention of the user who devotes it to one output item only; and PHOENICS cannot distinguish between intended and inadvertent inputs. Users are advised therefore first to take a 'bird's-eye view' of the simulated flow, and then to ask himself: "Do I believe this?"

Qualitative features of the flow should correspond with his expectations. Thus abrupt enlargements of the flow-cross-section should reveal recirculating-flow patterns downstream; and heavier fluids should fall below lighter ones. Most important is that the user should have expectations. If he does not he should ask a more experienced colleague. He must not (to repeat the important point already made) rely on PHOENICS to proclaim: "Something's wrong."

PHOENICS does, by default, print information about the numerical accuracy of the calculation. Thus the nett mass source, i.e. the difference between the inflow and the outflow, is printed in the RESULT file. The user is advised to inspect it.

2. Getting started

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:

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

  1. HELP Button on FLAIR VR-Environment Top menu.

    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.

  2. Bubble-help in VR interface hand-set.

    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.

  3. Help in the 2D-menu of the FLAIR VR and Object dialog boxes.

    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:

2.3 A simple example

2.3.1 Problem description

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:

  1. to start the FLAIR application with the default room
  2. to re-size the room
  3. to add objects to the room
  4. to activate the physical models
  5. to specify the grid number in each direction (the grid will be generated automatically) and specify solver parameters
  6. to calculate a solution
  7. to examine the results

The remaining sections provide step-by-step instructions on how to set up the model.

2.3.2 Setting up the model

Starting FLAIR

            

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.

2.3.2 Resizing the room

Figure 2.4 Resize the default room to 3mx5mx2.7m on the control panel

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

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

  1. Next add the wall at x = 0

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

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

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.

2.3.3 Running the Example

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:

Accessing the VR-Viewer

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:

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.

2.3.6 Summary

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 seven active HVAC-specific object types, Diffuser, Fire, Jetfan, Spray-head, Rain, Person, People and two post-processing objects ROOM_ACH and Raingauge as described below.

3.1.1 Diffuser

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) -

image104.gif (29618 bytes)

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.

3.1.2 Fire

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.

image100.gif (29245 bytes)

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:

image101.gif (11190 bytes)

Figure 3.12 Fire heat sources

Time,Qt
0,0
60,350000
120,700000
180,1050000
240,1400000
300,1400000
360,1400000
420,1400000
480,1400000
540,1400000
600,2055000

The 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:

Fire mass source options

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

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:

Fire scalar source options

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.

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.

3.1.3 Jetfan

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.

image88.gif (22234 bytes)

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.

3.1.4 Spray-head

The spray-head is the sprinkler designed for fire extinction. It works with the GENTRA 22 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/) / RTI
where 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 are correct, and no default settings will be made.

The settings made for GENTRA are:

3.1.5 Rain

The rain object in effect represents a rain-producing area of sky. It works with the GENTRA 22 module (see Encyclopaedia in POLIS). The rain object can be loaded through the Object management in the same way as described in section 3.1.1 above for the diffuser.

The default rain object and its attributes are shown in figure 3.16a below.

Figure 3.16a The default rain object

Each ball represents a GENTRA droplet injection port. Each port can emit up to five droplets of different diameters.

The attributes have the following meanings:

Number of ports (X) - sets the number of ports in the X direction.

Number of ports (Y) - sets the number of ports in the Y direction.

The rain object is assumed to be zero thickness in Z, and to extend in the X and Y directions. However, it can be freely rotated about the X, Y and Z axes from the object Place page. The shape is restricted to a rectangle.

Total rain flowrate - sets the rain flowrate from this object in mm/hr. The total flowrate is evenly distributed amongst all the droplet sizes from this object. Typical flowrates might be:

Number of droplet sizes - sets the number of droplet sizes emitted by each port. Up to five sizes can be specified. To specify more than one size, enter the required number of sizes and click 'Apply'. New input boxes will appear for the set number of sizes.

Diameters - sets the diameter(s) of each droplet in mm. The diameter of the first droplet size is initially deduced from the total rain flowrate using the expression:

Diam= 1.105*(Flow rate)0.232 (Ref 22)

Link airflow to tracks - the airflow will always affect the paths of the rain droplets. When this box is not ticked, it is assumed that the droplets do not influence the air flow. If it is ticked, then the full two-way interaction is implemented.

If GENTRA is not active at the time the first rain object is created, it will be automatically turned on, with all settings made for the rain model. Only the rain start- and end-times need be set for a transient case, should the rain not be active all the time.

If GENTRA is already turned on, it will be assumed that all settings are correct, and no default settings will be made.

The settings made for GENTRA are:

3.1.6 Person

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.

3.1.7 People

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

3.1.8 ROOM_ACH

The ROOM_ACH object is used to define a volume of space. The Earth solver will calculate the volume of the object, excluding any solid obstructions, and sum up the volumetric inflow rate across the boundary of the object, including any internal air supply. It will then print into the RESULT file the number of Air Changes per Hour for the volume defined by the object. It has no effect on the solution.

This is calculated from 3600.0*(sum of volumetric inflows)/(room volume).

A typical output is shown here:

 For object ACH_1       
 ---------------------
 Overall residence time calculated as
 free volume/volum.flow-rate (in seconds)
 RES.TIME=9.830783
 Ventilation rate in air changes per hour
 ACH =366.196655
 The total free volume in the room is (m^3)
 VOLUME =1639.037354
 The total volumetric flow rate is (m^3/s, m^3/hr)
 VFLRT s =166.725006 ;VFLRT h=6.0021E+05
 The total internal volumetric source is (m^3/s, m^3/hr)
 VFLRT s =10.000005 ;VFLRT h=3.600002E+04

The same information can be obtained in the Viewer by right-clicking on a ROOM_ACH object and selecting 'Show nett sources' from the context menu that appears. The data is then also written to a file called 'ACH results for object name at sweep n.txt', where name is the name of the object and n is the sweep number.

By default, the ROOM_ACH object is represented as a transparent cuboid, but it can be given any required shape, for example the CAD representation of the inside of a room.

3.1.9 Raingauge

The raingauge object is used to define a surface. The default shape is a cuboid, but any desired shape can be used. It counts the number of Rain tracks or Spray-head droplets passing through (only the entry point is noted), and reports the total mass passing through (entering) the object.

In the Editor, the Attributes dialog is not accessible. In the Viewer, the Raingauge attributes dialog appears as shown below:

Figure 3.18a The default Raingauge Dialog

To read a GENTRA particle history file, click 'Load'. If the history file has a non-default name, then first click GHIS and select the correct file before clicking 'Load'. Once all the tracks have been read in (this may take a little while if there are very many of them), the display will update showing all the tracks.

Figure 3.18b Typical image after loading tracks (Show All)

Initially, all loaded tracks are shown. To show only the tracks passing through the selected Raingauge object, toggle 'Show all' to 'Current'.

Figure 3.18c Typical image showing 'Current' tracks

Selecting another Raingauge will cause the screen to update to show the tracks passing through the newly-selected object.

Figure 3.18d Typical image showing 'Current' tracks

To display detailed information regarding the tracks, click 'Show net sources'. A window will appear displaying:

Figure 3.18e Typical 'Show results'

The same information is also written to a file named 'object_name.txt'. The 'Results' window can also be displayed by selecting 'Show net sources' from the right-click context menu of the selected Raingauge object.

3.2 The HVAC-specific objects and their default attributes

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.

The items supplied are provided as an example of what can be achieved. Users are encouraged to build up their own libraries of useful components, so that commonly-used items need only be defined once and can then be re-used in other projects. A simple tutorial on the creation of assembly objects is provided here.

3.2.1 Cabinets subdirectory contains the following object files:

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

  • 3.3.2 Object attributes

    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

  • 3.3.3 Exporting an Object

    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

  • 3.3.4 Object sizing, scaling and positioning

    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.

  • 3.3.5 Object Colouring and Rotation options

    The 'Option' button is used to change the colour of the imported object and to choose the rotation centre and rotation mode.

  • 3.3.6 Import custom geometry

    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.


  • 4. HVAC-Related Models

    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.


    5. References

    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 Boundary 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.

    18. A J Grandison, E R Galea, M K Patel. Fire Modelling Standards/Benchmark. Report on SMARTFIRE Phase 2 Simulations. Fire Safety Engineering Group, University of Greenwich, London SE10 9LS

    19. Stull, R. 2011 Wet-Bulb Temperature from Relative Humidity and Air Temperature, American Meteorological Society November 2011.

    20. Alduchov, O. A., and R. E. Eskridge, 1996: Improved Magnus form approximation of saturation vapor pressure. J. Appl. Meteor.,35,601-609.

    21. Steadman, R. G. 1973: The Assessment of Sultriness. Part II: Effects of Wind, Extra Radiation and Barometric Pressure on Apparent Temperature. Journal of Applied Meteorology, Vol 18, p874-885

    22. GENTRA User guide, CHAM TR/211.

    23. Blocken, B., Briggen, P.M., Schellen, H.L & Carmeliet, J., "Intercomparison of wind-driven rain models based on a case study with full-scale measurements", 5th Int.Symp. on Computational Wind Engineering, Chapel Hill, North Carolina, USA May 23-27, (2010).


    6. Tutorials

    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.


    Contents