Encyclopaedia Index

WORKSHOP - Use of Linked Angled Inlets.

This workshop example shows how two linked ANGLED-IN objects can be used to represent a duct that is not modelled.

The example is 2-dimensional. The fluid is air and the flow is turbulent and isothermal.

The geometry is to be as shown in the figure below, with the vertical dimension 1m and the horizontal dimension 2m :


wherein:

Preliminary remarks

  1. In addition to physically-meaningful data of the above kind, all CFD codes, and therefore PHOENICS also, require non-physical inputs such as:
  2. The non-physical settings suggested at first below are such as to make the calculations rapid rather than accurate.
  3. At the end of the tutorial, some further suggestions are made which will enable you to explore the influences of the settings on accuracy and speed of calculation.

Starting the tutorial

First activate the PHOENICS Satellite module in VR-Editor mode by either:

If you are uncertain of, or wish to change, your working directory, click on 'Options', 'Change working directory'.

In PHOENICS-VR Editor

When the Editor starts execution, what it shows on the screen will depend on what happens to be in your working directory. You can disregard this.

In order to make a fresh start;

You are now ready to begin.

Set the domain size, and activate solution of the required variables

Click on 'Main Menu' and set 'Linked Angled-In Objects' as the Title.

Click on 'Geometry'.

Change the X-Domain Size to 2.0 m and the Z-Domain Size to 1.0m.

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

Click on 'Models'.

Leave the 'solution for velocities and pressure' ON, and turn the Energy Equation ON. Select Temperature as the form of the Energy equation. The default turbulence model, KECHEN, can be left active.

Click on 'Top menu', then on 'OK' to exit the Main Menu.

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'.

reset1.gif (3045 bytes)

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 Block-1 object:

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

Change name to BLOCK-1

Click on 'Size' and set SIZE of object as:

Xsize: 0.2

Ysize: tick 'To end'

Zsize: tick 'To end'

Click on 'Place' and set Position of object as:

Xpos: 0.9

Ypos: 0.0

Zpos: 0.0

Click on 'General'.

Select Type: Blockage (default).

and on 'OK' to close the Object Specification Dialogue Box. BLOCK-1 will now appear in the Object Management list of objects.

Create the BLOCK-2 object:

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

Change name to BLOCK-2

Click on 'Size' and set SIZE of object as:

Xsize: 0.9

Ysize: tick 'To end'

Zsize: 0.1

Click on 'Place' and set Position of object as:

Xpos: 1.1

Ypos: 0.0

Zpos: 0.0

Click on 'General'.

Select Type: Blockage (default).

and on 'OK' to close the Object Specification Dialogue Box. BLOCK-2 will now appear in the Object Management list of objects.

Create the HEATER object:

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

Change name to HEATER

Click on 'Size' and set SIZE of object as:

Xsize: 0.2

Ysize: tick 'To end'

Zsize: 0.2

Click on 'Place' and set Position of object as:

Xpos: 0.35

Ypos: 0.0

Zpos: 0.0

Click on 'General'.

Select Type: Blockage (default).

Click 'Attributes'. Click Types and select 'Domain material'. This object will now be made of whatever material fills the domain (in this case air). It allows us to set heat sources.

Click Energy Source, and select 'Fixed heat Flux'. Enter 5000 in the Value box to set a heat source of 5000W for the entire object.

Clock 'OK' to close the Object Specification Dialogue Box. HEATER will now appear in the Object Management list of objects.

Create the OUT-L object:

Click on 'Object', 'New' and New Object'.

Change name to OUT-L .

Click on 'Size' and set SIZE of object as:

Xsize: 0

Ysize: 'To end'

Zsize: 'To end'

Click on 'Place' and set Position of object as:

Xpos: 0.0

Ypos: 0.0

Zpos: 0.0

Click on 'General'.

Define Type: OUTLET.

Click on then 'Attributes'. Set the external turbulence to 'User set'. The default user-set extarnal values give a turbulent viscosity which is roughly laminar. In many cases this is more stable than the 'In-cell' default setting which allows the external values to float.

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

Create the OUT-R object:

Click on 'Object', 'New' and New Object'.

Change name to OUT-R.

Click on 'Size' and set SIZE of object as:

Xsize: 0

Ysize: 'To end'

Zsize: 'To end'

Click on 'Place' and set Position of object as:

Xpos: 'At end'

Ypos: 0.0

Zpos: 0.1

Click on 'General'.

Define Type: OUTLET.

Click on 'Attributes'. Set the external turbulence to 'User set'. The default user-set extarnal values give a turbulent viscosity which is roughly laminar. In many cases this is more stable than the 'In-cell' default setting which allows the external values to float.

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

Create the INTAKE object:

Click on 'Object', 'New' and New Object'.

Change name to INTAKE.

Click on 'Size' and set SIZE of object as:

Xsize: 0.2

Ysize: 'To end'

Zsize: 0.2

Click on 'Place' and set Position of object as:

Xpos: 0.8

Ypos: 0.0

Zpos: 'At end'

Click on 'General'.

Define Type: ANGLED-IN.

Note that the shape and size of the angled-in object do not really matter - what matters is the size and shape of the area of intersection between it and any blockage which it overlaps. In this case the active inlet area will be the outer surface of the BLOCK-1 object which lies within INTAKE.

Click on 'Attributes' to set the inlet condition.

Enter 5.0 m/s for the velocity in the X-direction. This is pointing into the BLOCK-1 blockage and so will be treated as an extraction rate. In this case, the settings for temperature and turbulence do not matter, as it is the in-cell values which will be convected out. Click 'OK' to close the Attributes dialog.

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

Create the OUTLET object:

Click on 'Object', 'New' and New Object'.

Change name to OUTLET.

Click on 'Size' and set SIZE of object as:

Xsize: 0.1

Ysize: 'To end'

Zsize: 0.1

Click on 'Place' and set Position of object as:

Xpos: 1.55

Ypos: 0.0

Zpos: 0.05

Click on 'General'.

Define Type: ANGLED-IN.

Note that the shape and size of the angled-in object do not really matter - what matters is the size and shape of the area of intersection between it and any blockage which it overlaps. In this case the active outlet area will be the outer surface of the BLOCK-2 object which lies within OUTLET.

Click on 'Attributes' to set the inlet condition. We want to link the outflow here to the inflow calculated for INTAKE. INTAKe is the preceeding Angled-in in the list. Click on 'Link to other ANGLED-IN' until it states 'Previous'. Leave the additional heat source as zero, as we are assuming that there is no extra heating or cooling applied along the length of the notional duct linking INTAKE and OUTLET.

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

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.

Click anywhere on the image, and the 'Gridmesh settings' dialog box will appear.

The grid in all three directions is set to 'Auto'. This gives 20 cells in X and Z, and 1 cell in Y. This will suffice for the tutorial, though it would not be enough for a 'real' calculation. Click on 'OK' to close the dialog box. Click on 'Mesh toggle' again to turn off the mesh display.

Set the remaining solution-control parameters:

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

The default number of iterations is 100. This is enough to test if a model is set up correctly, but is hardly ever enough to obtain a converged solution.

Reset the total number of iterations to 300.

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

Click on 'OK' to exit the Main Menu.

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 in the middle of the right-hand airspace is fine. This will let us see if any flow is getting through from the other side of BLOCK-1.

Click on the probe icon on the toolbar or double-click the probe itself, and move the probe to X=1.5, Y=0.5, Z=0.5.

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).

Alternatively, click on the probe icon on the toolbar or double-click the probe itself to bring up the Probe Location dialog.

A typical vector and velocity plot from this case is:

The velocity from OUTLET is 10m/s which is double the velocity at which INTAKE is sucking. This is correct, as the area of OUTLET is half that of INTAKE.

A typical Temperature contour plot is:

To check the temperatures at INTAKE and OUTLET, first select INTAKE the right-click and select 'Show results'.  The Satellite command prompt will open showing the sums of sources for the INTAKE object.

Now do the same for OUTLET.

The mass flows (Nett source of R1, in kg/s) are equal and opposite, as expected. The energy sources (Nett source of TEM1 in W) are also opposite and equal and the average temperatures are the same.

Saving the results.

In the PHOENICS-VR environment, click on 'Save as a case', make a new folder called 'ANG-IN ' (e.g.) and save as 'CASE3' (e.g.). Return to the VR-Editor by clicking 'Run' - 'Pre-processor' - 'GUI Pre-processor'.