FLAIR Tutorial 1: Investigating library case I203

This tutorial is to illustrate how to load case I203, Ventilation of Hackney Hall from the FLAIR library and investigate its settings, run the case and view the results. However, this is a 3D real application and the user does not have to run through the case as it may take a few hours to complete.

Starting FLAIR with the default room

• Click the FLAIR icon (a desktop shortcut created by the FLAIR installation program); or
• Start the VR-Editor by clicking on 'Start', 'Programs', 'FLAIR', then 'FLAIR-VR'.
• Click on the 'File' button and then select 'Start new case', followed by 'FLAIR' and 'OK'.

The FLAIR VR-Environment screen should appear, which shows the default room with the dimensions 10mx10mx3m.

Loading the library case I203

• Click on the 'File - Load from libraries'. This will bring up the 'load from library' dialog as shown below

• If you If you know the number of the case you want to load, type it into the 'case number' data entry box and click OK
• Otherwise, click on 'Browse' and you will see the following dialog box

• Use the '+' next to Special-purpose programs to expand the library listings
• Click on 'Flair library' and 'Large cases'. Case I203 will be on the listings

• Select case I203 and click 'OK' to confirm the selected case number, and then OK to load it. There will be a display window which provides a link to the description. Click on the link, you will see the following details:

• The case was three dimensional, and the flow was steady.
• The geometry within the domain was created using PHOENICS-VR. As the auditorium was very nearly symmetrical, only half of the domain was modelled.
• The theatre includes balconies modelled as a series of stepped Cartesian blockages, and a new object was created to model the curved roof and stage.
• The computational domain is 33m long by 11.4m wide by 12.7m high, a 60*20*78 cells Cartesian grid was used, and PARSOL technique was used to map the non- Cartesian elements of the geometry; e.g. the curved roof and stage.
• The domain is filled with air, and ideal gas law was used in calculating pressure-temperature-density relationships. The roof, floors and walls were modelled using an adiabatic solid material.
• The effects of gravity were included by way of sources of momentum in the equations for the z component velocity using the built in buoyancy facilities available in PHOENICS.
• The Standard-KE model of turbulence is used to close the Reynolds-averaged Navier-Stokes equations.
• The air supply under the balcony, on the long side of the theatre, is introduced at 12degC. The incoming air velocity, from this long, slot is fixed at 3m/s, giving a mass flow rate of about 2.5m³/s.
• Further air is supplied under the seating, at the rear of the auditorium only, at 18degC. The inflow supply rate is 0.7m³/s, providing by seven 70mm high inlets.
• The occupant and light gains were modelled using heat sources respectively equivalent to 145W/m² and 50W/m².
• The ten outlets at the top of the domain were modelled as 500mm long by 250mm wide fixed pressure openings.

• You may close the window after viewing the description. After successful loading, the geometry of case I203 will appear on the screen as shown below

This case was to simulate the air flow and thermal characteristics in the theartre influenced by the ventilation system.

Investigating the model settings

• Click on the 'Object management' button, . You will see all the objects listed on the object management dialog box as shown below.

• You may double click on each of those objects and investigate their attributes. For example, you double click on object INLET3B (reference no. 36). This will bring up the 'Object specification' dialog box as shown below.

• Click on 'Attributes' button to bring up the 'Object attributes' panel as shown below. The settings show that the air is coming into the theatre at the speed of 0.16 m/s with the temeparture of 18 degree C.

• You can investigate the physical model settings by clicking on 'Main menu' button, and click on each model panel, for example 'Models' as shown below. As can be seen, the pressure, velocities and temperature are solved. The constant effective turbulence viscosity is used for the turbulence modelling.

Running the solver

• To obtain a solution for the loaded case, click 'Run - Solver' as shown below. Then click 'OK' to confirm.

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 solved variables at the monitoring point that was set during the model definition. The right-hand graph shows the variation of errors as the solution progresses.

A 3D real application like this requires about 30 minutes of computing time on a 3.5Ghz PC.

Viewing the results

• To run the Viewer, click on 'Run - Post processor - GUI post processor (VR Viewer)'.
• When the 'File names' dialog appears, click 'OK' to accept the current result files. You may use the 'Object management' dialog box to hide some of objects.
• Click on the 'T' (Select temperature) button, on the main control panel.
• Click on 'C', (select a variable) button, on the main control panel to bring up the 'Viewer options' dialog box as shown below

• Set the 'Maximum value' to 24 C. Tick 'Show contours'. The following contour plot should appear.

• Click on 'Streamline management' button, .
• Select 'Along line'
• Set the start point to X = 26; Y = 6.0; Z = 2.465.
• Set the end point to X = 26; Y = 11.0; Z = 2.465.
• Click 'Create Streamlines' to generate 15 streamlines staring an equal intervals along the specified line.
• Click 'OK' to close the 'Stream Options' dialog.

The following streamlines will be displayed on the screen.