Encyclopaedia Index

## WORKSHOP - In-Form: Time-varying Heat Source

### Overview

This example shows how to set a time varying heat source using In-Form. The case calculates the flow resulting from a car fire in a short tunnel. Note that in FLAIR, the heat source set here can be put in as a piece-wise linear source for a FIRE object without the need to use InForm.

The geometry of the case is shown in Figure 1 below. There are openings (outlets) at either end. The external temperature is 25°C.

Only half the tunnel width is represented, so there is a symmetry plane at y=0. The car geometry is only representative. The tunnel is inclined at 2°.

Figure 1. The geometry of the In-Form example

The heat source will be set to:

Q = min(10000*t, 3.0E6) for t < 720

Q = max(3.0e6-13000*(t-720), 5000) for t> 720

The heat source will thus increase linearly with time for the first 720 seconds, to a peak of 3MW which is reached after 300 seconds and maintained until 720 seconds. After 720 seconds, the heat source reduces linearly with time until it reaches a minimum value of 5kW at 950 seconds.

A complete step-by-step guide, showing how to set the case from the default mode of operation, is provided below.

### Accessing PHOENICS-VR.

From the system level:

To enter the PHOENICS-VR environment, click on the PHOENICS icon on the desktop, or click on Start, programs, PHOENICS, PHOENICS.

From the commander level:

To enter the PHOENICS-VR environment, click on the 'Run vre' icon in the left column.

In PHOENICS-VR environment,

Start with an 'empty' case - click on 'File' then on 'Start New Case', then on 'Core'', then click on 'OK'; to confirm the resetting.

To enter VR Editor:

This is the default mode of operation.

### Within VR Editor.

Set the domain size and grid numbers:

Click on 'Menu' (Main Menu) on the VRE-Editor panel (or the M icon on the tool bar); and then on 'Geometry'.

Set the x-domain size to 50.0.

Set the y-domain size to 5.0.

Set the z-domain size to 2.5.

Turn the 'Auto' settings for X, Y and Z to 'Manual', and set 'number of cells' to 40 in the x-direction, 5 in the y-direction and 20 in the z-direction. This is too coarse for an accurate solution, but will allow the tutorial to run relatively quickly.

Click on Time dependence 'Steady' to change to 'Transient'. Click on 'Time step settings'. Set the last time step number to 65, and the Time at end of last step to 1200s. Click on 'Split regions', and create a new region boundary at 10s. Set 10 steps for time region 1, and 55 for time region 2. This will make the first 10 steps 1s each, and the remainder to 21.6s. Click 'OK' to close the time step dialog. The change in time step size is probably too large, but illustrates the method of setting different step sizes.

Click on 'OK' to close the Grid mesh settings dialog.

The domain no longer fits the screen. To resize the view so that it does fit, click on the pull-down next to the 'R' icon on the toolbar then 'Fit to Window' and then repeat for 'View -Y'.

Models settings

On the Top Panel, enter 'Tunnel Fire' as the Title.

Click on 'Models'.

Leave 'Solution for velocities and pressure' at ON.

Switch 'Energy Equation' ON, and select 'Temperature'.

Click on Chen-Kim KE (Turbulence models) and choose Constant-effective. This is a very simple turbulence model used to make the tutorial run faster.

Physical properties

Click on 'Properties'. For the current domain material select 'Gases' - '2  Air using Ideal Gas Law STP'.

Note that the ambient pressure and temperature are 1atm and 20°C respectively. Set the Ambient temperature to 25°C.

'Initialise from ambient' is ON, so the initial values of pressure and temperature throughout the domain will be set to these values.

Initial Values

Click on 'Initialisation'. You will see that the initial values for P1 (pressure) and TEM1 (temperature) are both set to AMBIENT.

Set Whole-domain sources

Click on 'Sources'. Turn Gravitational forces ON. The Density-difference form will be activated.

The tunnel is to be tilted at 2° with Z pointing up. The Z component of gravity is therefore -9.81*cos(2). To tilt at 2° set the X component to -9.81*sin(2) which is -0.34. Set the components of the gravity vector to (-0.34,0.0, -9.804) in (x,y,z).

The reference density should be set to that at which the flow is neutrally buoyant - in this case 25°C.

On the Properties panel, 'Set buoyancy from ambient' was ON so the reference density has been set automatically from the ambient pressure and temperature. The value should be the density of air at 25°C, which is 101325/(287*(25+273)) = 1.1847 kg/m3.

Enter numerical settings

Click on 'Numerics'.

Set 'Total of number of iterations' to 50.

Set output controls

Click on 'Output', then on 'Settings' next to 'Write flow field'. Set 'Intermediate field dumps' to ON. Set the step frequency for dumping to 1, and the start letter for PHI (CSG1) to a. The Earth solver will write files called a1, a2, a3 and so on.

Click on 'Top menu' and then on 'OK' to exit from 'Menu'.

Create Objects and specify boundary conditions

Click on the 'Object Management' button (O on the toolbar or on the hand set). This will display a (currently empty apart from the domain) list of objects.

Create the openings

In the Object management dialog, click on 'Object', 'New' and 'New Object', 'Outlet' and select the X plane.

Change name to UP.

Set Position and Size of the object as:

Xpos: At end, Xsize: 0.0

Ypos: 0.0, Ysize: To end

Zpos: 0.0, Zsize: To end

Click on 'Attributes'

You will see that the External temperature is set to 'User-set' and the value is set to 'Ambient'. The external velocities are set to 0.0.

Click 'OK' to exit from the Object Dialogue Box.

In the Object management dialog, click on 'Object', 'New' and 'New Object','Outlet' and select the X plane.

Change name to DOWN.

Set Position and Size of the object as:

Xpos: 0.0, Xsize: 0.0

Ypos: 0.0, Ysize: To end

Zpos: 0.0, Zsize: To end

The default attributes will be as for the UP object, so do not need changing.

Click 'OK' to exit from the Object Dialogue Box.

Create the Roof Object

In the Object management dialog, click on 'Object', 'New' and 'New Object', 'Blockage'.

Change name to ROOF.

Set Position and Size of the object as:

Xpos: 0.0, Xsize: To end

Ypos: 0.0, Ysize: To end

Zpos: 0.0, Zsize: To end

On the 'Shape' tab, in 'Geometry', select public\shapes\corner. The new shape is not aligned correctly. Click on 'Options' then 'Rotation options'. The 'Rotate object face' entry sets the orientation of the shape within its bounding box. There are 24 possible orientations. Keep changing the orientation number until you find the one which makes the shape lie correctly (it is number 10). An alternative way to do the same job is to repeatedly click on the 'Rotate object up/down' buttons on the handset (if it is visible).

Click on 'OK' to exit the Rotation Options menu,

Click 'OK' to exit from the Object Dialogue Box.

Create the Ground plane

In the Object management dialog, click on 'Object', 'New' and 'New Object', 'Plate' and select the Z plane.

Change name to GROUND

Set POSITION and SIZE of object as:

Xpos: 0.0, Xsize: To end

Ypos: 0.0, Ysize: To end

Zpos: 0.0, Zsize:  0.0

Click on 'Attributes'. Set the Energy source to 'Surface Temperature'. Set the surface temperature to 25.

Create the Fire object

In the Object management dialog, click on 'Object', 'New' and 'New Object', 'Blockage'.

Change name to FIRE1.

Click on 'Geometry' on the 'Shape' tab. Open the folder 'public\Equipmt', and select 'car4' and click 'OK'.

Set the Size as:

Xsize: 4.7

Ysize: 2.0

Zsize: 1.3

We are only modelling half the tunnel, so the car can be placed so that one half is outside the domain.

Click on 'Options' and un-tick 'Object constrained by domain'. Set the Position as:

Xpos: 23.0

Ypos: -1.0

Zpos: 0.0

Click on 'Attributes' on the 'General' tab

Change the material type to 'Domain material'.

Click on 'In-Form Commands'. The Inform Sources dialog will appear.

Click the empty button under 'Keyword' and select SOURCE.

Click the empty button under 'Var' and select TEM1.

Click the empty button under 'Formula'. An editing window will appear. In the input window, type

`min(1e4*tim,3.e6)`

then click 'File', 'Save & Exit'.

Click the empty button under 'Condition'.  An editing window will appear. In the input window, type

`if(tim.le.720)!whol`

then click 'File', 'Save & Exit'. The 'whol' flag at the end of the statement states that the source is a total source for the whole object, not per-unit-volume.

Click the empty button on the second row under 'Keyword' and select SOURCE.

Click the empty button under 'Var' and select TEM1.

Click the empty button under 'Formula'. An editing window will appear. In the input window, type

`max(3.e6-1.3e4*(tim-720),5e3)`

then click 'File', 'Save & Exit'.

Click the empty button under 'Condition'.  An editing window will appear. In the input window, type

`if(tim.gt.720)!whol`

then click 'File', 'Save & Exit'. The In-Form Sources dialog should now look like this:

The easiest way of inserting these lines is to highlight them in the browser window, right-click and copy, then paste into the Save Block Editor window.

Click 'OK' to exit from the In-Form Sources dialog, then 'OK' to exit from the Object Dialogue Box.

Create a Point-History Object

Point_history objects can be used to 'instrument' the solution. At each Point_history object the time-histories of pressure, velocity and temperature will be written to the RESULT file. In the Object management dialog, click on 'Object', 'New' and New Object', 'Point_history'.

Change name to MONIT.

Set POSITION and SIZE of object as:

Xpos: 22.5 Xsize: 0.5

Ypos: 0.0 Ysize: 0.5

Zpos: 2.0 Zsize:  0.1

The actual size entered does not really matter, as it will be reset to fill the cell nearest the specified position.

All settings are now complete. The user should move the probe (small red pencil sign) to the position shown in Figure 1 (roughly x=22, y=0, z=2.2) before running the Solver, EARTH. Click on the probe icon on the toolbar or double-click the probe itself to move it.

### Running the Solver.

In the PHOENICS-VR environment, click on 'Run', 'Solver' then 'Local solver(Earth)', and click on 'OK'; to confirm running Earth.

### Using the VR Viewer.

In the PHOENICS-VR environment, click on 'Run', 'Post processor',then GUI Post processor (VR Viewer) Viewer)'. Click 'NO' next to Use intermediate step files and turn to 'YES'. Click 'OK' to accept starting with the file for step 1.

To view:

• Vectors - click on the 'Vector toggle'
• Contours - click on the 'Contour toggle'
• Streamlines - click on the 'Create Streamline' button
• Iso-surfaces - click on the 'Iso-Surface toggle'

To move on to the next time step, click or press F8. To go back one step, click or press F7. To jump to any other saved step, click or press F6. To cycle through all saved files, click the 'Animation' button.

Figure 2 shows the velocity vectors and temperature contours on the Y=0 plane after 312s.

Figure 2. Velocity vectors and temperature contours at 312s

Figures 3,4 & 5 show iso-surfaces of 250C at 118s, 312s and 853s

Figure 3. iso-surface of Temperature = 250°C after 118s

Figure 4. iso-surface of Temperature = 250°C after 312s

Figure 5. iso-surface of Temperature = 250°C after 853s

Figure 6 shows the time-history of temperature at the Point_history object MONIT. To get this image, select the MONIT object, right-click and select 'Show results'. Select TEM1 from the list of variables.

Figure 6. Time history of Temperature at MONIT

### Saving the results.

In the PHOENICS-VR environment, click on 'Save as a case', make a new folder called 'INFORM', select the new folder, and save as 'FIRE'.