Encyclopaedia Index

WORKSHOP - Flow Over Heated Bricks

Heat sources, Arraying

The following instructions will allow the user to set up and run the simulation of air in a cavity with heated bricks in VR.

The flow is three-dimensional and its geometry is shown below.

The geometry and simulation options are set up using VR Editor, the calculations are performed using the PHOENICS solver, EARTH, and the results are viewed using VR Viewer. Velocity, pressure and temperature will be simulated.

The initial and external temperature is 20 deg C. Buoyancy effects are significant due to the localised heating of the air around the blocks.

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.

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 activate solution of variables:

Click on 'Main Menu' and then on 'Geometry'.

Change the Z-Domain Size to 0.7 m.

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

Click on 'Models'.

Leave the 'solution for velocities and pressure' ON.

Click on 'energy equation' and

select 'Temperature' as energy formulation.

Click 'Properties'. Select '2 Air using Ideal gas Law, STP' as the domain material (it is in the Gases section).

Click 'Sources', and turn Gravitational forces ON. The Density_difference method will be automatically selected, and the Reference density will be automatically set from the ambient temperature and pressure on the Properties panel.

Click on 'Top menu' and then on 'OK'.

Click 'Reset' on the Movement control panel, then 'Fit to window' to re-scale the view to fit the geometry.

Create the objects making up the scene

Click on the 'Object Management' button (O on the toolbar or image172.gif (1000 bytes) on the hand set). This will display a (currently empty apart from the domain) list of objects.

Create the horizontal plate:

Click on 'Object', 'New', 'New object'.

Change name to PLATE.

Click on 'Size' to set the SIZE of object as:

Xsize: 0.7

Ysize: 0.9

Zsize: 0.01

Click on 'Place' to set the Position of object as:

Xpos: 0.15

Ypos: 0.05

Zpos: 0.19

Click on 'General'. The Type is Blockage (default).

Click on 'Attributes', then on 'Other materials', 'Solids' and select the material as STEEL.

Click on 'OK' to exit the Attributes menu and on 'OK' to exit the Object Dialogue Box.

Create the first brick:

Click on 'Object', 'New', 'New object'.

Change name to BRICK1.

Click on 'Size' to set the SIZE of object as:

Xsize: 0.1

Ysize: 0.05

Zsize: 0.05

Click on 'Place' to set the Position of object as:

Xpos: 0.15

Ypos: 0.45

Zpos: 0.2

Click on 'General'. The Type is Blockage.

Click on 'Attributes' and define the material as BRICK (go to OTHER MATERIALS, SOLID then to BRICK).

Click on 'Adiabatic', and select 'Fixed Heat Flux'

Set the heat flux to 30 W.

Click on 'OK' to close the Attributes menu.

Click on 'OK' to close the Object Dialogue Box.

Create the remaining bricks by arraying:

Check that the first brick built is still selected and appears with white contours, if not select it from the list in the Object management Dialog.

Now click on the 'Duplicate using array button', or select 'Object', 'Array object' from the Object Management Dialog menu bar. In either case, in the new dialogue box, set

Direction Dimension Pitch
X 4 0.2
Y 1 0.0
Z 1 0.0

Click on 'OK' to exit from the Array Dialogue Box.

A row of bricks with the same attributes appears in the domain.

Create the fluid inlet;

Click on 'Object', 'New', 'New object'.

Change name to INLET.

Click on 'Size' to set the SIZE of object as:

Xsize: 0.4

Ysize: 0.5

Zsize: 0.0

Click on 'Place' to set the Position of object as:

Xpos: tick 'at end'

Ypos: tick 'at end'

Zpos: 0.0

Click on 'General' and define Type: Outlet.

Click on 'Attributes' to define the external conditions.

Set the External turbulence to 'User-set' and leave the default values. This will give a turbulent viscosity roughly the same as laminar.

Leave the temperature at ambient, 20 degrees C for the inflow.

Click on 'OK' to close the Attributes menu, and on 'OK' in the Object Dialogue Box.

Create the fluid outlet:

Click on 'Object', 'New', 'New object'.

Change name to OUTLET.

Click on 'Size' to set the SIZE of object as:

Xsize: 0.4

Ysize: 0.5

Zsize: 0.0

Click on 'Place' to set the Position of object as:

Xpos: 0.0

Ypos: 0.0

Zpos: tick 'at end'

Click on 'General' and define Type: Outlet.

Leave the default values in the Attributes dialogue box.

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

Setting the Probe Location

Before running the solver, it is a good idea to place the probe in a suitable place to monitor the convergence of the solution. Too close to an inlet, and the value will settle down very quickly before the rest of the solution. Placed in a recirculation zone, it may still show traces of change even though the bulk solution is converged. In this case, somewhere under the dividing plate is fine.

Click on the probe icon on the toolbar or double-click the probe itself, and move the probe to X=0.5, Y=0.5, Z=0.3

Set the grid

Click on the 'Mesh toggle' button. The default mesh will appear on the screen. The orange lines are region lines, and denote the edges of the bounding boxes of each object. The blue lines are ordinary grid lines introduced by the auto-mesher.

The auto-mesher actually does quite a good job in the X-Y plane, but leaves the grid coarse at the domain edges in the Z direction. For a real calculation, we would refine the grid in X and Y, making sure there were more cells in the gaps around the edges of the plate. For now, we will refine the grid at the Z-direction domain edges.

Click anywhere on the image, and the 'Gridmesh settings' dialog box will appear. The grid in all three directions is set to 'Auto'.

Click 'Edit all regions in Z direction', and set Boundary - Low and High both to 'On'. This will make the grid in the first and last regions use a symmetrical power law. The number of cells should reduce from 46 to 35. Click 'OK' twice to close the grid dialogs.

The final mesh should look like this

Set remaining solution control parameters:

In the Main Menu, click on 'Numerics'.

Set the number of iterations to 500. This is still not quite enough for a fully-converged solution, but will give a good idea of the flow.

Click on 'Top menu' to return to the top menu.

Click on 'OK' to exit the Main Menu.

Running the Solver.

In the PHOENICS-VR environment, click on 'Run', '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) . Click 'OK' on the file names dialog to accept the default files.

To view:

To select the plotting variable:

To change the direction of the plotting plane, set the slice direction to X, Y or Z slice direction (927 bytes)

To change the position of the plotting plane, move the probe using the probe position buttons

probe position (927 bytes).

A typical plot from this case is:

Note that the top value on the temperature scale has been reduced to emphasise the thermal plume rising from the right-hand brick.

A typical streamline plot is shown here.

The streamlines were started 'around a circle' of radius 0.1, with the Probe at (0.8,0.75,0.01) and the plotting plane set to Z.

Saving the results.

In the PHOENICS-VR environment, click on 'Save as a case', make a new folder called 'BRICKS' (e.g.) and save as 'CASE1' (e.g.).