Encyclopaedia Index

Contents list

VR Object Types and Attributes

Object Type

Transient Cases
Start and End Times Transient Heat Sources Transfer Objects

InForm Commands

Weather data for WIND and SUN objects

This chapter describes the object types, and their attributes. The attributes of each object type are specific to that type. They are set by clicking the 'Attributes' button on the Object Specification 'General' page.


Object Type

The allowable object Types are:


Image: TYPES

Object Type Brief Description
Blockage 3D, solid or fluid. Can apply heat and momentum sources.
Inlet 2D, fixed mass source.
Angled-in 3D, fixed mass source on surface of underlying BLOCKAGE object.
Wind 3D, whole domain, applies wind profiles at domain boundaries
Wind_Profile 2D, fixed mass source following atmospheric boundary layer.
Outlet 2D, fixed pressure.
Angled-out 3D, fixed pressure on surface of underlying BLOCKAGE object.
Sun 3D, whole domain, applies solar radiation heat load within domain.
Plate 2D, zero thickness obstacle to flow. May be porous.
Thin Plate 2D, nominal thickness for heat transfer.
Fan 2D, fixed velocity
Point_history single cell transient monitor point.
Fine Grid Vol 3D region of fine grid.
User Defined 2D or 3D, for setting user-defined sources (PATCH/COVAL).
Celltype  2D or 3D, for setting user-defined sources (cannot affect grid).
Null 2D or 3D. Used to cut the grid for mesh control.
PCB  3D, solid or fluid with non-isotropic thermal conductivity
Pressure Relief single cell fixed pressure point.
ROTOR 3D, rotating co-ordinate zone in cylindrical-polar grid
Drag_lift 3D, region over which momentum imbalance (force) will be calculated.
Assembly 2D or 3D container object for multi-component object
Transfer 2D, transfers sources between calculations
Clipping_plane 3D, graphically clips the image. No effect on solution.
Plot_surface 2D or 3D, provides surface for contour or vector plots in Viewer. No effect on solution.

Many of the object types have a set default geometry. These are listed in the relevant sections below, and are mainly cuboids of different colours. If a geometry which is not a cuboid is selected, then this will not be changed.

An internal consistency check is performed to ensure that the object dimensionality and selected object type are consistent. VR-Editor will not allow a 2D attribute for a 3D object, or vice-versa.

Each object type may have different attributes; these are set by clicking on the Attributes button.


Blockage

A blockage is a volume object, which may prevent flow within itself. The default blockage material, 198 Solid with smooth-wall friction, also prevents any heat transfer within the blockage. In effect, any region occupied by such a blockage does not exist as far as the calculations are concerned.

The default geometry for a solid blockage is shapes\cube14.dat. This is a grey cuboid.

Clicking on the Attributes button for a blockage brings up the following dialog box:

Image: ATTRIBUTES DIALOG BOX

  1. Blockage Material

    The material a blockage is made of is set by clicking on 'Other Materials', which brings up the material type dialog box.

    Image: OTHER MATERIAL DIALOG BOX

    Selecting any of the material classes will bring up a further list of the available materials of that class. The list is read from the central property file, usually stored as \phoenics \d_earth \props. Any materials added to this file by the user will be available for selection.

    If the Material of the blockage is changed to that of a 'real' solid, then the object will participate in the heat transfer calculations, should they be active, but will remain blocked to flow. If the object is made from a gas or liquid, then it will participate completely.

    It is also possible to select 'Domain fluid' as the material for a blockage. This will automatically pick up whatever material has been specified in the properties panel of the main menu. A typical use of this is to 'drill' a hole through another solid. The 'drilling' object must come after the object it is making a hole in. The object order can be changed from the Object Management Dialog by right-clicking in the 'Reference' column.

    Once the solid is participating in the solution, additional buttons appear which allow heat sources to be specified (if applicable). Initial values for temperature can also be set. If the blockage material is a gas or fluid, then momentum and scalar sources can be specified. Initial values can be set for pressure, velocity and solved-for scalars. Porosity values in each co-ordinate direction can be specified.

    If the material is a gas or liquid, the default geometry is changed to shapes\cubet.dat, which is a transparent cuboid. If a heat source has been activated, the default geometry becomes shapes\cube4.dat for solids, and shapes\cubet1.dat for gases and liquids. These represent solid red and transparent red cuboids respectively.

  2. Blockage Roughness

    By default, solid blockages pick up the global surface roughness set in the Main Menu - Sources panel. An individual roughness height for the current object can be set.

    Image: OBJECT ROUGHNESS SETTING

  3. Blockage Wall Function

    By default, solid blockages pick up the auto wall-function coefficient set in the Main Menu - Sources panel. An individual wall-function coefficient can be set. The options are:

    Image: OBJECT WALL-FUNCTION COEFFICIENTS

    For a friction-less blockage, material 199 Solid allowing fluid-slip at walls must be selected. This material also prevents heat transfer within the blockage.

    If a Wind or Wind_profile object is also being used, the wall function on any plate used to represent the ground should be set to 'Fully rough', and the roughness height set to the same value as was used for the wind velocity profile.

  4. Blockage Slide Velocity

    This option only appears for solid blockages, but not for blockages made from a fluid. By default the surfaces of the blockage are stationary. It is possible to set a non-zero surface velocity. The options for Cartesian grids are:

    IMAGE: Slide Velocity Options

    For polar grids, the options are:

    IMAGE: Polar Slide Velocity Options

    The Z-direction component is always the axial velocity in m/s.

    Note that these options do not cause the object to move relative to other objects and no convective effects are allowed for inside the object - they just impart moving boundary conditions on the outer surface. It is as if the object were covered with a rubber belt which was moving in the prescribed way.

  5. Blockage Energy Sources

    If the energy equation is solved, then for any participating material, the following types of energy source can be selected by clicking on the Energy source entry box labeled Adiabatic:

    Images: ENERGY SOURCES

    These are defined as:

    Fixed temperature: The temperature throughout the volume of the object is fixed to the set temperature

    Fixed Heat Flux: The heat flux throughout the volume of the object is fixed to the set value. The value can be specified as a total flux for the object, or as a flux per unit volume. (units W or Wm3)

    Adiabatic: There is no heat source. This is the default setting for a new object.

    Linear Heat Source: The heat source in any cell within the object is calculated from the expression

    Q = Vol * C (V - Tp)    (units of C - W/m3/K or W/m3/C, units of V - K or C)

    where C and V are user-defined constants, Tp is the local cell-centre temperature, and Vol is the cell volume.

    Quadratic Heat Source: The heat source is calculated from the expression

    Q = Vol * C (V - Tp)2    (units of C- W/m3/K2 or W/m3/C2, units of V - K or C)

    User Defined Source: The heat source is calculated from the expression

    Q = Vol * C (V - Tp

    where C and/or V are calculated in the user's open-source GROUND routine and Vol is the cell volume.

    The units of temperature are determined by the setting of the Reference Temperature on the Main Menu - Properties panel. If this is set to 0K, the unit of temperature is degrees Kelvin. If it is set to 273K, the temperature unit is degrees Celsius.

    If the blockage is the default cuboid non-participating material, heat sources can still be applied to its exposed faces.

    If IPSA is on, energy sources are set separately for each phase.

  6. Blockage External Heat-Transfer Coefficient The blockage heat source defined in the previous section for participating solids sets the heat source within the blockage itself. Heat-transfer between the blockage and the surrounding fluid is controlled by the blockage external heat-transfer coefficient.

    By default, this is obtained from the wall-functions. Alternatively, a user-set constant value can be supplied.

    Image: BLOCKAGE HEAT TRANSFER COEFFICIENT

    The values of heat transfer coefficient used can be stored into the PHI file for plotting in the Viewer. This is done from the Main Menu - Output - Derived Variables panel.

  7. Blockage Momentum Sources

    If the pressure and velocities are solved for, and the blockage is a gas or liquid, the following types of momentum source can be selected independently for each co-ordinate direction:

    Image: MOMENTUM SOURCES

    Fixed Velocity: The velocity throughout the volume of the object is fixed to the set value.

    Fixed Momentum Flux: The momentum flux (force) throughout the volume of the object is fixed to the set value. The value is specified as a total force in Newtons for the object.

    None: There is no driving force. This is the default setting for a new object.

    Linear Source: The force in Newtons is calculated from the expression

    F = mass-in-cell * C (V - Velp)   (units of C - 1/s, units of V - m/s)

    where C and V are user-defined constants, and Velp is the velocity in any cell within the object.

    Quadratic Source: The force is calculated from the expression

    F = mass-in-cell * C (V - Velp)2   (units of C - 1/m, units of V - m/s)

    This form is suitable for representing distributed pressure losses which obey dP = K *density * velocity2, where K is an empirical constant, set as C.

    User Defined Source: The force is calculated from the expression

    F = mass-in-cell * C (V - Velp)

    where C and/or V are calculated in the user's open-source GROUND routine

    If IPSA is on, momentum sources are set separately for each phase.

  8. Blockage Scalar Sources

    If additional scalar variables (e.g. C1) are solved, and the blockage is a gas or liquid, the following types of source can be selected for any solved scalar equation:

    Image: SCALAR SOURCES

    Fixed value: The scalar throughout the volume of the object is fixed to the set value.

    Fixed Flux: The flux throughout the volume of the object is fixed to the set value. The value can be specified as a total flux for the object, or as a flux per unit volume.

    None: There is no scalar source. This is the default setting for a new object.

    Linear Source: The source is calculated from the expression

    S = Vol * C (V - fp)    (units of C - 1/(sVolf))

    where C and V are user-defined constants, fp is the scalar value in any cell within the object, and Vol is the cell volume.

    Quadratic Source: The source is calculated from the expression

    S = Vol * C (V - fp)2     (units of C - 1/(sVolf2))

    User Defined Source: The source is calculated from the expression

    S = Vol * C (V - fp)

    where C and/or V are calculated in the user's open-source GROUND routine.

  9. Blockage Initial Values

    Initial values can be set for temperature, pressure, velocity, solved scalars and cell face and cell volume porosity factors.

    If the Simple Chemically-reacting System (SCRS) is active, and an initial temperature has been set, the corresponding initial gas composition must be set as well.

    If IPSA is active, initial volume fractions for Phase 1, Phase 2 and the Shadow phase (if solved) can be set.

    If Algebraic Slip is active, initial particle concentrations can be set.

    If either of the free-surface models, SEM or HOL, is active, the blockage can be designated as being either heavy or light fluid.

    In all cases, if the Initial value button is left as No, the initial value for that quantity will be that set in the Initialisation panel of the Main Menu. If Initial value is set to Yes for pressure or temperature, the default initial value is the ambient value set on the Properties panel of the Main Menu. This can be changed to user if some other value is required.

  10. Blockage Emissivity

    If the IMMERSOL radiation model is active, the emissivity of a solid, or the absorption and scattering coefficients of a gas or liquid, can be set.

  11. InForm Commands

    This leads to a dialog from which a selection of InForm commands can be attached to this object. It is described in InForm Commands below.

  12. Solar Absorption Factor
  13. When a SUN object is active an additional input box appears, in which the fraction of the incident solar radiation absorbed by this object can be set. The default absorption factor is 1.0 - i.e. all the heat is absorbed by the object. For most substances absorption is 0.5 or greater; bricks, weathered steel and marble can be up to 0.9. The exceptions are polished metal surfaces -typically .1-.2.


Inlet

An inlet is a region of fixed mass flow, either in or out. Inlets can only be attached to area objects.

The sign convention for velocities is that a velocity pointing in to the domain brings mass in, whilst a velocity pointing out takes mass out. For volumetric flow rate, positive flow is in to the domain, negative flow is out.

The default geometry for an inlet is shapes\cube3t.dat, which is a transparent purple cuboid.

  1. Single phase

    The basic single-phase inlet dialog box for turbulent flow is shown below:

     

    Image: SINGLE PHASE DIALOG BOX

    Acts as: Export / Import allows the inlet object to behave as a Transfer Object. When Export is activated, an input box for the export file name appears. The default is the current object name. At the end of the Solver run, the named file will be created, and it will contain the mass flows and other values for all cells covered by the object.

    If Import is activated, the remaining attributes are hidden, as the inflow conditions will be read from a file. The file name can either be entered into the input box, or searched for with a file browser. The default is also the current object name.

    The Nett area ratio sets the ratio between the area actually available for flow, sometimes called the effective area, and the area used in the model. If the ratio is less than 1, the actual injection velocity or volumetric flow rate should be specified for the inlet condition. The mass flow will be calculated from area_ratio*velocity*density.

    A density is required to calculate the mass flow rate. If the 'Inlet density is' is set to Domain fluid, the density will be taken from the formula selected for the domain fluid in the Main Menu, Properties panel. The density will be calculated from the values set at the inlet. For compressible flows, the pressure (used to calculate the density) can be the ambient pressure set in the Main Menu, Properties panel, or a user-set value.

    If the fluid entering is not the domain fluid, the setting can be switched to User-set, as shown below. In this case, the required inlet density can be set directly. (This is the default for complex density relationships).

    The inlet Temperature (only present if the Energy Equation is active) can be switched between Ambient and User. When set to Ambient, the inlet temperature is always taken from the Ambient Temperature set on the Main Menu, Properties panel. When set to User, any required value can be entered.

    The Method button switches between:

    For polar grids, the options for Method are:

    If the flow is turbulent, the turbulence quantities at the inlet can be deduced from a turbulence intensity, or they can be directly specified by the user. This is controlled by the Inlet turbulence button.

    When the 'Intensity' method is chosen, the inlet values of k and e are calculated from:

    kin = (0.01*I*Vnorm)2

    ein = (Cm*Cd)3/4* kin3/2/(0.1*len)

    where:         I is the turbulence intensity in %;

    Vnorm is the velocity normal to the inlet; and

    len      is the length scale, taken to be the hydraulic radius of the inlet. This is half the hydraulic diameter, which is calculated from 4*area/perimeter. The area and perimeter are always based on the bounding box of the object, so may not be accurate for a non-cuboid shape. In BFC cases len is the equivalent radius, calculated from (area/p)1/2

    Cm, Cd  are constants in the turbulence model, defaulted to 0.5478 and 0.1643 respectively. These values can be changed from the Main Menu, Models, Turbulence Models, Settings panel.

    Note that the 'Intensity' method is suitable for duct-type flows. Atmospheric boundary layers should be treated as described below for Wind_Profile Objects.

    If the inlet values of k and e are known, then the User-set method should be selected and the known values entered.

    Inlet values for solved scalars are set by selecting the scalar with the Setting scalar button, then specifying the required inlet value.

    Image: FLUID SETTING

    If the SCRS combustion model is on, a button appears which allows the inlet gas composition to be set. The enthalpy at the inlet is then deduced from the inlet temperature, gas composition and gas properties.

    Note that if the reaction type is switched from mixing-controlled to kinetically-controlled, or vice-versa, the inlet gas composition values will have to be reset.

  2. Multi-phase

    If IPSA is active, a new button appears, which allows a switch between setting values for Phase 1 or Phase 2. The Inlet density button toggles between Phase fluid and Dens*Vol frac. Phase fluid indicates that the density will be that of the current phase. Dens*Vol frac indicates that the value entered is the product of density and volume fraction.

    If only one phase enters, all three velocity components or flow rates of the absent phase should be set to zero.

    If Algebraic Slip is on, the Inlet density button toggles between Mixture density and User-set. Mixture density means that the inlet density will be calculated from the densities of the various particle phases and the set inlet concentrations.

    If the free-surface models SEM or HOL are on, the Inlet density button toggles between Heavy fluid and Light fluid. SEM and HOL do not allow mixtures of phases at an inlet.

    If the Lagrangian Particle tracker GENTRA is active, Inlets can be set to act as particle exits.

  3. Radiative Heat Loss

    If the IMMERSOL radiation model is active, the inlet can be allowed to exchange heat by radiation with the surroundings. If the External radiative link is set to Yes, the temperature of the surroundings, Texternal, can be set. The heat flux from the inlet will then be:

    Q" = s (Text4 - Tp4)   (W/m2)

    where s is the Stefan-Boltzmann constant.

  4. Internal Inlets

    If the inlet is internal to the domain, an extra button appears on the dialog box, labeled Object side. The settings for this are Low or High, and they indicate whether the inlet is to appear on the low-co-ordinate face or high-co-ordinate face of the object. The flow direction determines whether the inlet acts as a source or sink, as shown in the table below.

      Low High
    Inflow -ve velocity +ve velocity
    Outflow +ve velocity -ve velocity

    When inside the domain, INLET objects are usually located on the face of a BLOCKAGE. They represent the outflow (or inflow) from some ducting inside the blockage that is not being modeled. Positive velocity always points along the positive coordinate direction. The 'Object side HIGH/LOW' setting determines whether it represents an inflow or outflow, as in the table above.

                      --------
                     |        |
                ---->|Blockage|---->
                     |        |
                      --------
                    L H      L H
    
                     ---------> X, Y or Z

    If the setting is 'LOW', as on the left side above,  the inlet acts on the smaller-coordinate side of the inlet. A positive velocity points into the blockage and thus acts as a fixed-extraction zone. If the setting is 'HIGH',as on the right side above, the inlet acts on the larger-coordinate side, and a positive velocity points out into the domain and acts as a supply. A negative velocity reverses the situation, making the left side a supply and the right an extraction.

    If the setting is HIGH on the left side or LOW on the right side, the inlet acts inside the blockage and nothing happens at all.

    With volume or mass flow rates, the sign convention is easier, in that positive flows are always inflow to the domain, and negative flows are always outflow from the domain.


Angled-In

An Angled-in is a region of fixed mass flow, either in or out. The region of influence is the part of the surface of any blockage object(s) enclosed by the angled-in object. The angled-in object itself must be a 3D volume.

The sign convention for velocities is that a velocity pointing in to the domain brings mass in, whilst a velocity pointing out takes mass out. For volumetric flow rate, positive flow is in to the domain, negative flow is out.

The default geometry for an angled-inlet is shapes\cube3t.dat, which is a transparent purple cuboid.

The angled-in object may intersect a blockage, as shown here:

IMAGE: Angled-in intersects blockage

It may also completely surround a blockage, as shown here:

IMAGE: Angled-in surrounds blockage

Its area of influence cannot lie on the domain edge, as it must interact with a blockage.

The attributes of the Angled-in object are as those of the 'normal' inlet, with the addition of 'Normal velocity' to the methods of specifying the flow rate. This sets the velocity normal to the surface of the underlying blockage. It was used in the second example above to make the flow issue radially from the cylindrical blockage.

If the 'Intensity' method is chosen for the turbulence quantities, the inlet values are calculated from:

kin = (0.01*I*Vnorm)2

ein = (Cm*Cd)3/4* kin3/2/(0.1*len)

where:         I is the turbulence intensity in %;

Vnorm is the velocity normal to the inlet; and

len      is the length scale, taken to be the equivalent radius of the inlet. This is   calculated from (area/p)1/2. The hydraulic radius cannot be estimated as the perimeter is unknown in this case.

Cm, Cd  are constants in the turbulence model, defaulted to 0.5478 and 0.1643 respectively. These values can be changed from the Main Menu, Models, Turbulence Models, Settings panel.

If the inlet values of k and e are known, then the User-set method should be selected and the known values entered.

Linked Angled-ins

In order to represent the flow through a piece of equipment which is not modelled in detail but is represented as a blockage, it is possible to use a pair of linked Angled-in objects.

For example, to represent an Induction Fan, one Angled-in can be used to represent the suction side of the fan. Here the extraction flowrate is specified. The nozzle of the fan is then a second Angled-in, linked to the first.

The mass flow will be taken from the first, and the temperature and other scalars will be the average values at the first. The velocity at the outflow will be deduced from the mass flow rate and the area of the outlet. If the density is set to use the Ideal Gas Law, the outlet density will be evaluated at the average outlet temperature.

linked angled-ins

The image shows the smoke ingested by the lower intake Angled-in being ejected by the nozzle Angled-in.

In a similar way, ducting can be represented by using one Angled-in (acting as an extract) as the inlet to the duct, and a linked Angled-in as the outlet from the duct. This is demonstrated in the Tutorial ' Working with Linked Angled Inlets'.

An Angled-in can be linked to the immediately-preceding or immediately-following Angled-in. The linked Angled-ins do not need to be adjacent in the Object Management list.

Once linked, an additional heat source can be specified, representing any extra heating or cooling taking place.

Limitations

Linked Angled-ins have the following limitations:


Wind

Dialogs, Weather Data, Radiative heat loss, Transient operation, Initialisation, GENTRA, Wind Amplification factor

The initial WIND attributes dialog is shown here:

WIND dialog

IMAGE: WIND Dialog

The WIND object is very closely related to the WIND_PROFILE object described below. In steady state, only one WIND object is allowed, and it always fills the entire domain. Based on the wind direction it creates inflow boundaries at the domain edges using logarithmic or power law profiles on the upwind faces, and fixed pressure boundaries on the downwind (and side) faces. In addition, the upper, or sky boundary can also be made into a fixed pressure boundary and the appropriate friction conditions can be applied to the floor plane.

In transient cases, multiple WIND objects are allowed on the basis that their start- and end-times do not overlap. This gives the possibility to allow the wind direction and / or speed to change with time. However, if a weather file is being used, a single WIND object will pass all the required time-varying data to the solver.

The formulae used to calculate the velocity and turbulence quantities as a function of height are given below.

The items on the dialog are as follows:

Use weather data file. When set to No, as shown above, the user must supply all the required input data as set out below. When set to Yes, the input data are taken from an EnergyPlus EPW weather data file. The method for doing this is described in the section 'Loading a Weather Data File' below. The data in the weather file can also be used by a SUN object to supply the solar heating load. WIND and SUN always use the same weather file, and will use data for the same date and time.

External density. The external density is used to calculate the mass inflow. It can be taken to be the same as the domain material density, or set to a user-specified value. If the domain density is a function of pressure (and/or temperature), the External pressure (and/or External temperature) will be used to evaluate it.

External pressure. This sets the pressure outside the domain. It is taken to be the same at all open faces. It may be used to calculate the inlet density. The external pressure is the atmospheric pressure at the edges of the domain. The reference pressure (PRESS0) is reset to this value. The reference pressure can be seen on the 'Main Menu - Properties' panel. The Ambient pressure seen on the 'Main Menu - Properties' panel is set to zero.

When a weather file is in use, the external pressure is taken from the weather file.

On the downwind, fixed pressure, faces, the pressure is set to zero relative to the reference pressure, which has been automatically set to the external pressure.

Coefficient. This controls how closely the internal pressure at the down stream boundaries (and upper boundary if Sky is active) approaches the set external pressure. When set to Linear, the mass flow through the pressure boundaries is a linear function of pressure difference. A fairly large value of the order of 1000 will keep the internal pressure very close to the external, suppressing any internal pressure gradients at the boundaries. When set to Quadratic, the coefficient represents a loss in dynamic head across the boundary. The mass flow is proportional to the square root of pressure difference. A small number should be used to reduce the pressure loss. See the entry on Coefficient in the Outlet object description below for more details.

Temperature. This sets the ambient temperature outside the domain. It is specified as the external value at all the faces, and may be used to calculate the inlet density. The Ambient temperature seen on the ' Main Menu - Properties' panel is reset to the external temperature. This, together with resetting the reference pressure to the external pressure, enables the reference density used for buoyancy to be set equal to the density at the external pressure and temperature.

When a weather file is in use, the external temperature is is taken from the weather file.

Wind speed. This sets the absolute value of the wind velocity in m/s at the reference height. When a weather file is in use, the value is taken from the weather file.

Wind direction. This sets the direction that the wind is blowing from. There are sixteen pre-set directions of North, North-North-East, North-East, East-North-East, East, East-South-East, South-East, South-South-East, South, South-South-West, South-West, West-South-West, West, West-North-West , North-West and  North-North-West.

To specify any other direction, select 'User' and enter the required angle in degrees, relative to North. A value of zero means that the wind is blowing from due North. The angle increases clockwise to 90 for East, 180 for South and 270 for West. Any value in the range -360.0 to 360.0 is valid. When a weather file is in use, the direction is set to File, and the value is taken from the weather file.

The wind direction is always relative to North.

WIND object

IMAGE: WIND object representation

The blue arrow points to North, and the red arrow shows the direction the wind if blowing from, in this case from the North.

Reference height. This sets the height at which the Wind Speed is specified.

Angle between Y (or X or Z) axis and North. This, and the Vertical direction determine the orientation of the domain with respect to North. With the angle set to zero,

In the example below, increasing the angle will rotate the North-facing axis (i.e. Y) clockwise when looking down along the vertical axis (i.e. Z):

winddir.gif (8648 bytes)

This allows the domain to be oriented conveniently with respect to a building or group of buildings.

Profile type. The boundary layer velocity profile can be a logarithmic or power-law function of height above the ground. This is measured from the first open cell.

Vertical direction. This controls which axis will be pointing up. The options are Z, Y or X. It is not possible to make the vertical axis point downwards.

Effective roughness height. This sets the roughness height at the edge of the domain. Typical values are given below. Values can be selected from a list, or a user-set value can be entered.

Surface type Roughness height zo (m) Power-law exponent a
Open sea 0.0002 0.16
Open flat terrain, grass, few isolated obstacles 0.03 0.13
Low crops, occasional large obstacles 0.10 0.16
High crops, scattered obstacles 0.25 0.19
Parkland, bushes, numerous obstacles 0.50 0.21
Suburb, forest, regular large obstacle coverage 0.50 to 1.0 0.21 to 0.24

It is advisable to set the roughness height of the object used to represent the ground to the same value, and to set the wall-function type to 'Fully-rough' to ensure that the wind profiles are maintained within the domain. This value should not be greater than the height of the first cell-centre above the ground.

Include open sky. When set to No, the upper boundary is treated as a frictionless impermeable lid. When set to Yes, the upper boundary is treated as a fixed pressure boundary. The external pressure, pressure coefficient and temperature are the same as at the down wind boundaries. The free stream velocities and turbulence quantities are calculated from the boundary layer formula at that height above the ground. In addition, the diffusive link between the top cell and the free stream value is activated. This helps to preserve the boundary layer profile.

Include ground plane. When set to No, the ground plane is left as a frictionless adiabatic surface. It is up to the user to provide an appropriate boundary condition, by using a PLATE object to represent flat terrain, a BLOCKAGE object to represent undulating terrain or a combination of these. The 'Wall function law' for these objects should be set to 'Fully rough', and the roughness height set to the same value as that used for the inlet profiles.

When set to Yes, a ground plane with the appropriate wall function and roughness height settings will be created to cover the whole of the bottom face of the domain.

Solar absorption factor. When the ground plane is included, the 'Solar absorption factor' determines how much of the incident solar radiation is absorbed.

Ground Temperature. When the ground plane is included, the ground surface can be adiabatic or fixed surface temperature. This temperature is set by the user. If a weather file is in use, the value is taken from the weather file. If other thermal conditions are required, the ground plane can be turned off, and a PLATE object used instead.

Radiative Heat Loss

If the IMMERSOL radiation model is active, the domain boundaries can be allowed to exchange heat by radiation with the surroundings. If the External radiative link is set to Yes, the temperature of the surroundings, Texternal, can be set. The heat flux from the wind profile boundary will then be:

Q" = s (Text4 - Tp4) (W/m2)

GENTRA particle Tracker

If the Lagrangian Particle tracker GENTRA is active, the domain boundaries will act as particle exits by default. This can be switched off.

Transient operation

When a weather data file is not being used, the operating time of the WIND object can be set as for most other objects. A number of WIND objects can be created with consecutive start and end times, each with different flow conditions. This way the time variation of wind speed and direction can be accommodated.

When a weather data file is being used, the situation is simpler. The date and time chosen represent the time at the start of the calculation. The time-varying data is extracted from the weather file and is passed to the Earth solver automatically. Only one WIND object is needed.

Initialisation

If the initial values for the velocities are all left at their default values of 1E-10m/s, the WIND object will impose initial conditions based on the chosen boundary layer formula, shown below for the WIND_PROFILE object.

If the initial values of the turbulence quantities KE and EP are left at their default values of 1E-10m/s, the WIND object will impose initial conditions based on the logarithmic profile.

The values used by the WIND object are echoed to the RESULT file, as in this example:

************************************************************
 Wind profile data
 -----------------
 Up direction Z
 Inlet density 1.204938E+00 kg/m^3
 Reference height 1.000000E+01 m
 Roughness height 1.000000E-01 m
 Profile type - Logarithmic Law
 Pressure coeff at outflow boundaries 1.000000E+03
 Wind direction 9.000000E+01
 Wind speed 1.000000E+01 m/s
 Air temperature 2.000000E+01C
************************************************************

Wind Amplification factor

When 'Store Wind Amplification Factor' is set to 'Yes', an additional 3D variable called WAMP will be STOREd, and the solver will fill it with values of the local air velocity divided by the set wind speed.

Restrictions

The following restrictions apply to the wind object:

The WIND object always fills the entire domain. Once the user is certain that it is oriented correctly, it can safely be hidden, or made wire-frame so that it does not obscure the objects within the domain. An alternative is to make it not selectable, so that the internal objects can be picked from the screen. The WIND object can always be selected from the Object Management Dialog


Wind_Profile

wind.gif (38293 bytes)

IMAGE: WIND_PROFILE dialog

The inlet boundary conditions associated with a wind velocity profile (the atmospheric boundary layer) can be specified by using a WIND_PROFILE object. Either a logarithmic or power-law velocity profile can be specified, as follows:

U/U* = ln(z/zo )/ k

U/Ur= (z/zr)a

and the turbulence quantities are set to:

k = U*2/0.3;   e= U*3/(k*z)

where U is the total velocity at the height z from the ground; k is von Karman's constant (=0.41), zo is the effective roughness height of the ground terrain; Ur is the reference velocity at the reference height zr, and a is the power-law exponent. The total friction velocity U* is given by:

U*= Ur k/ln(zr/zo)

Typical values of the roughness height zo and the power-law exponent a are given in the table below:

Surface type Roughness height zo (m) Power-law exponent a
Open flat terrain, grass, few isolated obstacles 0.03 0.13
Open sea 0.0002 0.16
Low crops, occasional large obstacles 0.10 0.16
High crops, scattered obstacles 0.25 0.19
Parkland, bushes, numerous obstacles 0.50 0.21
Suburb, forest, regular large obstacle coverage 0.50 to 1.0 0.21 to 0.24

The roughness height should not be greater than the height of the first cell-centre above the ground as this may lead to numerical problems.

The reference height zr is usually taken as 10m because this is the height at which mean wind data are generally provided. Engineers often prefer to use a power law profile, although the log law is to be preferred because it is based on physical laws rather than on an empirical formulation. A commonly-used empirical relationship between a and z0 is:

a = 0.096 log10 (zo) + 0.016 [log10 (zo)]2 + 0.24

The height above the ground, z, is measured from the first open cell in each column of cells. This allows the profile to follow the terrain imposed by a blockage.

IMAGE: Wind profile starting over a terrain

A density is required to calculate the mass flow rate. If the 'Inlet density is' is set to Domain fluid, the density will be taken from the formula selected for the domain fluid in the Main Menu, Properties panel. The density will be calculated from the values set at the boundary location.

If the fluid entering is not the domain fluid, the setting can be switched to User-set. In this case, the required inlet density can be set directly. (This is the default for complex density relationships).

Inlet values for solved scalars are set by selecting the scalar with the Setting scalar button, then specifying the required inlet value.

Radiative Heat Loss

If the IMMERSOL radiation model is active, the wind profile boundary can be allowed to exchange heat by radiation with the surroundings. If the External radiative link is set to Yes, the temperature of the surroundings, Texternal, can be set. The heat flux from the wind profile boundary will then be:

Q" = s (Text4 - Tp4) (W/m2)

Internal Wind profiles

If the wind profile boundary is internal to the domain, an extra button appears on the dialog box, labeled Object side. The settings for this are Low or High, and they indicate whether the inflow is to appear on the low-co-ordinate face or high-co-ordinate face of the object. The flow direction determines whether the boundary acts as a source or sink.

GENTRA Particle Tracker

If the Lagrangian Particle tracker GENTRA is active, the wind profile boundary will act as a particle exit by default. This can be switched off.

Restrictions

The following restrictions apply to the wind_profile object:

InForm Commands

This leads to a dialog from which a selection of InForm commands can be attached to this object. It is described in InForm Commands below.


Outlet

An outlet (also referred to as an OPENING in Flair) is a region of fixed pressure. Outlets can only be attached to area objects. The flow direction is actually unspecified, and depends on local pressure differences, although usually the flow will be out of the domain.

The default geometry for an outlet is shapes\cube12t.dat, which represents a transparent light-blue cuboid.


Angled-out

An Angled-out is a region of fixed pressure. The region of influence is the part of the surface of any blockage object(s) enclosed by the angled-out object. The angled-out object itself must be a 3D volume. The flow direction is actually unspecified, and depends on local pressure differences, although usually the flow will be out of the domain.

The default geometry for an angled-out is shapes\cube12t.dat, which represents a transparent light-blue cuboid.

The angled-out object may intersect a blockage, as shown here:

IMAGE: Angled-out intersects blockage

It may also completely surround a blockage, as shown here:

IMAGE: Angled-out surrounds blockage

Its area of influence cannot lie on the domain edge, as it must intersect a blockage.

The attributes of the Angled-out object are as those of the 'normal' outlet, with the addition of 'Normal velocity' to the methods of specifying the external velocity. This sets the velocity normal to the surface of the underlying blockage.


Sun

Dialogs, Weather Data, Transient operation, Absorption of solar radiation by objects, Additional output, Limitations

The SUN object applies the direct and diffuse solar radiation heat load to objects within the domain, taking into account:

Solar radiation perpendicular to the sun's rays at the top of the earth's atmosphere has an annual mean irradiance of approximately 1370 W/m2, with a seasonal variance of around +/- 3.5W/m2. In passing through the atmosphere, part of this energy is absorbed by the atmosphere, part is scattered by the atmosphere - some back into space and some to the earth (the diffuse 'sky' radiation), and the remainder (direct radiation) is transmitted through the atmosphere unchanged.

There are many sources available from which values of the direct and diffuse radiation may be obtained. One such source is the collection of weather data files from the U.S Department of Energy, freely available as part of the EnergyPlus Energy Simulation Software. Weather data for more than 2100 locations are now available in EnergyPlus weather format 1042 locations in the USA, 71 locations in Canada, and more than 1000 locations in 100 other countries throughout the world. The weather data are arranged by World Meteorological Organization region and Country.

The sun object can use these weather data files directly to obtain the direct and diffuse solar radiation at a particular date and time of day. The WIND object can also read the weather data file to obtain the wind speed and direction, and the temperature of the air and ground.

The default SUN dialog is shown here.

SUN dialog

IMAGE: SUN dialog

Get North and Up from WIND. When set to No, the user must specify the orientation of the domain relative to North. When set to Yes, the orientation is shared with the (first if more than one) WIND object (which must have been created already). When shared with WIND, the input box on the SUN dialog is grayed out, and any change in domain orientation must be made on the WIND dialog. This ensures that the SUN and WIND are oriented identically eliminating a potential source of error.

Angle between Y axis and North. This works in the same way as for the WIND object. It allows the domain to be oriented conveniently with respect to a building or group of buildings.

SUN Object
IMAGE: SUN Object

The orange arrow points North. When 'Get NORTH and UP form WIND' is set to Yes, the orange arrow is not drawn as it is then the same as the WIND's blue arrow.

In the example below, increasing the angle will rotate the North-facing axis (i.e. Y) clockwise when looking down along the vertical axis (i.e. Z):

winddir.gif (8648 bytes)

Use weather data file. When set to No, as shown above, the user must supply all the required input data as set out below. When set to Yes, the input data are taken from an EnergyPlus EPW weather data file. The method for doing this is described in the section 'Loading a Weather Data File'. The data in the weather file can also be used by a WIND object to supply the inflow/outflow conditions at the domain boundaries.  SUN and WIND always use the same weather file, and will use data for the same date and time.

Latitude. This sets the latitude of the location. The Equator is at 0 degrees, the Northern hemisphere is 0 to 90 (at the North pole), and the Southern is 0 to -90 (at the South pole). If a weather file is in use, this is set to the value read from the weather file.

Direct Solar radiation. This sets the incident solar radiation in W/m2. In the EnergyPlus data sets this is referred to as the Extraterrestrial Direct Normal Radiation. If a weather file is in use, this is set to File and the value is taken from the weather file.

If a weather file is not in use, it can be set to Constant or From solar altitude. In the latter case  the direct solar radiation is obtained from polynomial fits to tables A2.24 (direct) and A2.25 (diffuse) of The CIBSE Guide, Volume A Design Data. These give the following values in W/m2:

Solar Altitude
 (degrees)
Direct Radiation
Normal to Sun (W/m2)
Diffuse Radiation (W/m2)
Clear Cloudy
5 210 25 25
10 390 40 50
20 620 65 100
25 690 70 125
30 740 75 150
35 780 80 175
40 815 85 200
45 840 90 225
50 860 95 250
60 895 100 300
70 910 105 355
80 920 110 405
90 930 115 455

The solar altitude is obtained from the sun direction vector as calculated either at the start of the run, or at the start of each step in a transient.

Diffuse Solar radiation. This sets the diffuse solar radiation in W/m2. If a weather file is in use, this is set to File and the value is taken from the weather file. If a weather file is not in use, it can be set to Constant or From solar altitude, in which case values are interpolated from the table above, with the solar altitude calculated from the latitude, date and time of day. The further setting Clear sky or Cloudy sky determines which column to use.

Date. This sets the date (Day, Month, Year) at which the sun position is calculated. Strictly only the day and month are important. If a weather file is in use, this entry is taken from the weather file.

Time. This sets the time of day (using the 24 hour clock) at which the sun position is calculated. The time here is in effect local time, not taking any daylight-saving into account. At 12:00 (noon) the sun is at its highest position. If a weather file is in use, this entry is taken from the weather file.

In the image above, the large orange ball marks the sun position at the current time of day. The small orange balls denote the sun position on the hour during the day, and the grey balls at night when the sun is below the horizon. The red ball denotes the sun position at midday. The orange line drawn from the current sun position to the middle of the ground plane shows the direction of the sun's rays.

Optional extra output

There are several optional settings which can help to show how the model is working. These are activated from the 'Optional extra output' dialog:

Sun optional output

Consider the following simple example, in which the sun is shining from the front to the back.

Illumination example

The following 3D variables can be stored:

SRF distribution

LIT distribution

There is one cell near the top of the block which appears illuminated, but is on the back face of the central block. The centre of this cell can still see the sun.

#QS2 distribution

 In this image the suspicious cell can be seen to have only the diffuse heat source, as the face is pointing away from the sun.

When plotting these variables in the Viewer it is best to turn the contour averaging off, otherwise the averaging process will introduce values of SRF and LIT between 0 and 1 which do not exist. The heat sources only exist in a single layer of cells, so the averaging will appear to dilute them.

Transient operation

In a transient case, the time that should be set is the time at the start of the calculation. At each time step, the position of the sun will be adjusted, and the shading and resulting heat sources recalculated.

If a weather data file is in use, the radiative loads at each time in the data file are passed to the Earth solver. The solver will perform a linear interpolation between these values to find the value at the current calculation time.

If a weather file is not in use, the solar radiation can either be a constant, or can be derived from the solar altitude as described above. The solar altitude will be automatically updated for each time step.

Further settings

Absorption of Solar Radiation by Objects

When the SUN object is active, an extra input appears on the dialogs of BLOCKAGE, PLATE and THIN PLATE objects. This sets the amount of incident solar radiation absorbed by that object. The default absorption factor is 1.0 - i.e. all the heat is absorbed by the object. For most substances absorption is 0.5 or greater; bricks, weathered steel and marble can be up to 0.9. The exceptions are polished metal surfaces -typically .1-.2.

For participating blockages the solar energy is deposited in the outer-most layer of cells in the blockage. From there, the heat can be conducted away into the center of the blockage, as well as being convected and radiated away from the surface.

For non-participating blockages (.i.e. those using the 198 or 199 materials) and for plates, the solar energy is deposited in the layer of fluid cells adjacent to the object.

Echo of Settings

The settings in use by the sun object are echoed into the RESULT file by the solver, as shown in this example:

  ************************************************************
   Solar Heating data
   ------------------
   Latitude 51.00
   Time of day JUN 01 15:00:00 2011
   Constant direct solar heating 5.000000E+02 W/m^2
   Constant diffuse solar heating 1.000000E+02 W/m^2
  ************************************************************
  ************************************************************
   Solar altitude: 4.400269E+01
   Direct solar radiation: 5.000000E+02 W/m^2
   Diffuse solar radiation: 1.000000E+02 W/m^2
  ************************************************************

Limitations

The shading calculation is very dependent on there being enough grid to resolve sufficient detail of the geometry. If the grid is too coarse the illumination and resulting heat sources will be inaccurate.

The shading algorithm only works with Z as the UP direction.

The SUN object always fills the entire domain. Once the user is certain that it is oriented correctly, it can safely be hidden, or made wire-frame so that it does not obscure the objects within the domain. An alternative is to make it not selectable, so that the internal objects can be picked from the screen. The SUN object can always be selected from the Object Management Dialog.


Plate

A plate is a blockage, which can be treated as having zero thickness. This allows for computational efficiency, because complete cells do not have to be blocked, only cell faces. There is no heat transfer by conduction through a plate.

The default geometry for a plate with no heat sources is shapes\cube11.dat, which represents a brown rectangle.


Thin Plate

This is similar to the PLATE type, except that heat transfer through the plate is allowed. A notional thickness and material type are specified, but these are only used for the calculation of thermal resistance.

The object must be an area. Thin plates are only allowed within the domain, but not at the edges. The default geometry for a Thin Plate is shapes\cube11.dat, a brown rectangle.

The Thin Plate dialog box is shown below:

Image: FULLY BLOCKED 'YES'

If 'Fully blocked' is changed to 'No', the porosity can be set to be greater than 0.0.

Image: FULLY BLOCKED 'NO'

The velocity and pressure drop formulations are as for the PLATE object.

If the Energy Equation is on, the initial temperature of the plate can be set.

If the IMMERSOL radiation model is on, the surface emissivity for either side of the plate can be set.

Solar Absorption Factor. When a SUN object is active an additional input box appears, in which the fraction of the incident solar radiation absorbed by this object can be set. The default absorption factor is 1.0 - i.e. all the heat is absorbed by the object. For most substances absorption is 0.5 or greater; bricks, weathered steel and marble can be up to 0.9. The exceptions are polished metal surfaces -typically .1-.2.

Separate absorption factors are specified for each side of the thin plate.


Fan

When located at the domain edges, a FAN behaves as an INLET - it acts as a source of mass. If it is located within the domain, it fixes the velocity, but does not introduce additional mass - it just circulates the fluid already present. For multi-phase flows, Fans at the domain edge must be replaced by INLET objects. Fans can only be attached to area objects.

The default geometry for a Fan is shapes\cube2t.dat, a transparent grey rectangle. The domain-edge Fan dialog box is shown below:

Image: DEFAULT FAN ATTRIBUTES

The Nett area ratio sets the ratio between the area actually available for flow, sometimes called the effective area, and the area used in the model. If the ratio is less than 1, the actual injection velocity or volumetric flow rate should be specified for the inlet condition. The mass flow will be calculated from area_ratio*velocity*density.

The Fan can be switched between Velocities and Vol. Flow rate, as for Inlets.

A circular fan object can be created by clicking on Change to circular fan with swirl. Circular Fans are not available in Cylindrical-polar or Body-Fitted co-ordinates.

Image: CIRCULAR FAN ATTRIBUTES

The circular Fan allows for swirl, and for an inner radius. If the inner radius is zero, the entire surface of the Fan is active. If it is not zero, the Fan becomes an annular Fan with a central hole.

The swirl direction is set clockwise or anti clockwise looking along a positive co-ordinate direction. The Swirl Number is the ratio between the tangential velocity and the axial velocity. (It is the tangent of the Swirl Angle.) The tangential velocity is taken to be constant across the fan radius.

The default geometry for a circular Fan is shapes\cylpipe.dat.

A circular fan forces region boundaries at the axis, and at the location of the inner radius, giving a 4*4 grid in general.

If a circular Fan is located internally, the areas outside the active zone of the Fan are open to flow. If it is necessary to block them, an extra object with the geometry shapes\cylinder.dat can be used to fill the central hole, and four further objects using shapes\hh1.dat in appropriate orientations to fill the four corners.

Image: CIRCULAR FAN + FILLERS

If either Fan type is given a non-default geometry, the flow conditions will be imposed over those cells covered by the facets of the geometry file.

If the Lagrangian Particle tracker GENTRA is active, Fans can be set to act as particle exits.

The equivalent internal-fan dialogs are shown here:

Image: INTERNAL FAN DIALOGS

InForm Commands

This leads to a dialog from which a selection of InForm commands can be attached to this object. It is described InForm Commands below.


Point_history

This object type is used in transient calculations to mark locations at which time-histories are required. Any combination of SOLVEd and STOREd variables can be monitored. By default, values of pressure (P1), the three velocity components (U1, V1 and W1) and the temperature (TEM1) will be saved.

Time histories of selected variables are stored in the RESULT file. The cell monitored is the one whose centre lies closest to the probe location (Xpos, Ypos, Zpos). The time histories can then be plotted in the VR-Viewer by selecting a Point_history object, right-clicking it and choosing 'Show result' from the context menu.

The object does not affect the grid.


Fine Grid Vol

This volume object type is used to denote regions within which the grid is to be refined. The attributes dialog box sets the grid refinement ratios in each of the co-ordinate directions.

Image: OBJECT ATTRIBUTES

Fine grid volumes may be embedded within each other as deeply as required, with the constraint that each 'child' volume can only have one 'parent' - one volume cannot overlap two others, although they may touch at their boundaries.

Earth will disallow attempts to refine in directions in which the main grid has only one cell.

The default geometry for a fine grid volume is shapes\fine.dat.

Note that fine grid volumes are not compatible with:


User Defined

This allows any user-defined PATCH to be attached to an object. The Lecture on Boundary Conditions, and the Encyclopaedia entries on PATCH, COVAL and TYPE give more details on what settings to make. The default geometry is default.dat, a light brown cuboid.

Image: UNIVERSAL OBJECT ATTRIBUTES

To create a new patch, click on New, and enter a name, up to seven characters long. Click on Apply to create the patch. Click on Type, and enter the patch type, e.g. HIGH or NORTH. Finally, click on the Coefficient and/or Value slots required, and enter the values.

As many Patches as required can be attached to a single object. Clicking on PATCH number will cycle through the available Patches. The > (and <) symbol next to Variable scrolls through the list of available variables, if there are more than five.

The object can be an area or a volume.

Note that if the object type is changed from user_defined to some other type, a dialog will appear offering to delete any patches declared. This should be done, otherwise they will remain in the Q1 file.


Celltype

This is like the User Defined object, except that instead of forcing the grid to match the faces of the object, any related source is applied to the cells whose centres happen fall within the object. It is frequently used to define a fixed-pressure cell in a closed volume. The default geometry is default.dat, a light brown cuboid.


Null

This denotes an area or volume object introduced solely for the purpose of grid control. It has no effect on the calculation, other than creating additional grid regions. The default geometry is shapes\wirexyz.dat. This is a wire-frame outline of the bounding box.


PCB

The PCB (Printed Circuit Board) object behaves as a Blockage, with the exception that:

The default geometry for a PCB is shapes\cube1.dat, a green cuboid.


Pressure Relief

The Pressure Relief object is used to create a fixed-pressure point, usually in an enclosed domain. It does not affect the grid - the cell whose centre is nearest the position is used as the fixed-pressure cell.

The only attributes are pressure coefficient and value. Value is the pressure to be fixed, relative to the reference pressure set in the Properties panel of the Main Menu. Coefficient fixes how closely the pressure in the domain matches the set value. A coefficient of 1000 is often found to work well.

Note: The pressure-relief object does not affect the grid. The size of the object is adjusted on exit from VR to cover the cell nearest the origin of the object.

The default geometry for a Pressure Relief object is shapes\cubet.dat, a transparent grey cuboid


ROTOR

A ROTOR object represents a zone of rotating co-ordinates in a cylindrical-polar grid. Within the scope of this object, the grid is rotating about the Z axis with a set speed. Here, additional sources are added to the X- and Y-direction velocities to account for the centrifugal and Coriolis forces associated with the rotation.

Any BLOCKAGE objects falling within the scope of the ROTOR object will rotate with the rotor. A typical use for this object type is to model a rotating fan or impeller.

The advantage of this over the whole-domain rotating co-ordinates activated from the Sources panel is that the objects within the ROTOR can move relative to other stationary objects.

Image: ROTOR Object dialog (for transient case)

The dialog for the ROTOR object sets the following items:

As U1 (and U2) is relative to the rotating co-ordinates within the ROTOR object and relative to the stationary co-ordinates in the rest of the domain, it is not meaningful to plot vectors using it.

In the Viewer, the vector components should be chosen as U1RL,  Y-Velocity, Z-Velocity for vectors relative to the ROTOR, or TRU1, Y-Velocity, Z-Velocity for vectors relative to the domain.

Setting time steps for transient cases

When the ROTOR attributes dialog is closed, a second dialog opens, asking whether to set the time-steps from the settings made.

Image: ROTOR Time-step settings

The number of steps is calculated from:

LSTEP = ROTS * NX * 2p / (NJUMP*XULAST)

and the duration from:

TLAST = 60. * REVS / ROTS

If 'Cancel' is pressed, the time grid will be left as it is. In that case it is up to the user to ensure that the time steps, grid size and rotation speed are all consistent.

Multiple ROTORs

Multiple ROTOR objects are allowed, with the following restrictions:

  1. ROTOR objects cannot overlap in the Z direction, and must be separated by at least one plane of cells in Z.
  2. The rotation speed ROTS can only be set for the first ROTOR object. The rotational speed of subsequent ROTOR objects is directly linked to that of the first by the number of cells jumped each step.
    ROTSi = ROTS*NJUMPi/NJUMP1

    If the second or subsequent ROTOR is to rotate slower than the first, then the first must jump by more than one cell per timestep.

  3. ROTORs can rotate in opposite directions.

Restarting transient ROTOR cases

To restart a calculation in order to do further revolutions, e.g. calculate revolutions 4-6 having already calculated 1-3:

  1. On the ROTOR Attributes dialog of the first ROTOR, change the number of rotations to 6. Close the dialog, and allow the time steps to be set for 6 revolutions.
  2. Go to Geometry, 'Time step settings' and change 'First step number' to the number of steps in the first run plus one. If the first 3 revolutions took 100 steps, enter 101. Allow the restart to be activated, and check that the deduced restart file names are as expected.
  3. Run the Solver.

To restart from an intermediate step, say step 50, just set 'Number of first step' to 51 on the 'Time step settings' dialog and allow the restart to be activated. Check that the name of the restart file has been set to A50 (assuming that the start letter had been set to A). Click on 'Restart for all variables' to activate the restart, then run the Solver.

Further points to consider

The default geometry for a Rotor object is shapes\polcubt2.dat, a transparent light grey annulus which follows the polar grid.


Drag_lift

The Drag_lift object has no attributes. It defines a volume over which a momentum balance will be performed. The pressure, convection and diffusion fluxes are summed over the six faces of the bounding box of the object. The resulting force is printed to the RESULT file if 'Output of forces and moments' has been set to 'On' in the Main Menu - Output panel.


Assembly

The assembly object has no attributes of its own. It acts as a 'container' for any number of other objects. Objects are added to an Assembly from the 'Hierarchy' button of the Object Dialog General page.

Image: Object Hierarchy Dialog

The 'Add components' button is the only one present for a new Assembly. It brings up a list of objects, from which the components can be selected. The 'List' button shows the names of the current components, and 'Remove components' removes selected objects from the component list.

Once an object has been made a component of an assembly, its individual 'Size' and 'Place' pages are disabled. The 'Size' and 'Place' pages for the assembly affect all the components of the assembly. The size and initial position of the assembly object should be set before any components are added.

To move a component of an assembly relative to the other components, select the component, and from the General page select Hierarchy. 'Disconnect' from the Assembly and close the Object dialog. The 'Size' and 'Place' pages will reappear the next time the Object dialog is opened. Make any changes required, then select Hierarchy again and 'Make into a component' to reattach to the Assembly object.

All the objects in an Assembly can be exported to a single file, for use in other models. This is done from the 'Export' button of the General page. The exported file, known as a POB (Phoenics Object) file, will be saved to the current working directory. To make it available in other projects using other working directories, copy it to a sub-directory of \phoenics\d_satell\d_objects\users.

To import a saved Assembly, click on 'Object', 'New' 'Import Object'. Browse for the required POB file and select it. POBs can be imported from the local working directory, or from sub-directories of \phoenics\d_satell\d_object. All the component objects in the POB file will be imported. During the import process, a dialog will appear showing the position of the assembly, as read from the POB file. This can be changed as required at this stage, or the assembly can be moved later.

Note the following restrictions:

As mentioned above, the components of an assembly must have higher sequence numbers than the assembly object. If the assembly object is, for whatever reason, created after the components, the objects must be re-ordered before the components can be added to the assembly.

To do this, open the Object Management Dialog. Select the assembly object to be moved, and right-click in the 'reference' column. Using 'Line up' or 'Page up' or 'Top', move the object until it appears above all the component objects. Now proceed to add components to the assembly as normal.


Transfer

A Transfer Object can either:

Images:

Default dialog

Export dialog

Import dialog

Transfer objects are part of the domain-partitioning technique, in which a large domain which is too large to model accurately on one computer is divided into a number of smaller domains, each of which can be handled by one computer. Each domain is solved in turn, starting with the most upwind ones. The technique is limited to cases where the flow is predominantly uni-directional.

At the end of each calculation, data describing the flow conditions on the downstream boundaries are placed into files which serve as 'transfer objects'; for the data can then be imported as upstream-boundary data for the later-to-be simulated next-downstream part.

As Transfer Objects are commonly placed at the same location as inlets and outlets, the Inlet and Outlet object types can also export and import the flow data thus removing the need for duplicate objects. A single Transfer Object can of course cover several inlets and outlets.

Current limitations are:


Clipping_plane

Clipping plane objects can be created and manipulated in the Editor or Viewer.

Each Clipping_plane object consists of 3 OpenGL clipping planes. A maximum of two such objects are allowed, as there are only 6 clipping planes. The first Clipping plane object is created at the origin, and clips everything 'behind' it. This is the left-hand object above. The second Clipping plane object is of type 'High end clipping plane' (on the Options tab), and is originally located at the far end of the domain This is the right-hand object above. It clips everything 'after' it. They can be moved and rotated at will to provide a better view inside objects or to remove (from view) items obscuring the are of interest.

Clipping plane objects can also be created from 'Settings - New - Clipping plane' on the Environment Settings menu, or 'Object - New - Clipping plane' on the Object Management Dialog. When created in the Editor, they will be written to the Q1 like all other objects whenever the Q1 is saved. When created in the Viewer, they will persist if the Editor is entered from the Viewer, but disappear if exit is to the system as Viewer never saves the Q1.

Clipping plane objects never affect the grid, and have no influence on the solution.


Plot_surface

Plot surface objects can be created and manipulated in the Editor or Viewer, but their primary role is to aid visualisation in the Viewer.

They can be any size and any shape. Once created, the Viewer can plot contours or vectors on the surfaces of the object.

Plot_surface objects can also be created from 'Settings - New - Plotting surface' on the Environment Settings menu, or 'Object - New - Plotting Surface' on the Object Management Dialog. When created in the Editor, they will be written to the Q1 like all other objects whenever the Q1 is saved. When created in the Viewer, they will persist if the Editor is entered from the Viewer, but disappear if exit is to the system as Viewer never saves the Q1.

Plot_surface objects never affect the grid, and have no influence on the solution.


Transient Cases

  1. Start and End Times

    If the case is transient, additional settings will appear on many of the above dialog boxes. A typical example is shown in the Inlet dialog box below:

    Image: ADDITIONAL SETTINGS

    Active all the time Yes indicates that this inlet will be active for the entire duration of the transient. If Yes is toggled to No, the dialog box changes as shown below:

    Image: INLET DIALOG BOX

    The start and end times can now be entered. For the Earth run, the source will start in the time step which begins at, or closest to, the set start time and will end on the time step which ends at, or closest to, the set end time. Care should be taken to ensure that the time step settings will match the start and end times to a sufficient degree.

    Note that the same time limits apply to all sources from a single object.

  2. Transient Heat Sources

    In a transient case, the following additional heat sources (marked by the vertical line) can be set, either for a blockage or a plate:

    Image: ENERGY SOURCE

    Typically, these extra time-varying sources require four additional settings. These are shown in the portion of the dialog box below, for Value step of time:

    Image: VALUE STEP OF TIME

    This will produce a heat source of the form:

    Image: TEMPERATURE OR HEAT FLUX

    The extra settings have the following meanings:

  3. Transfer Objects

In a transient case, the name entered for either the export or import file is used as a base, and the time step number is appended before use. One file is written or read for each transfer object for each time step.

This is true whether the transfer is initiated from an Inlet, Outlet or Transfer Object.

Inform Commands

Many objects types have a button labeled 'InForm Commands' on their attributes page. This leads to a dialog from which a selection of InForm commands can be attached to the current object. The usual format of an InForm command is as follows:

(KEYWORD of VARIABLE at LOCATION is FORMULA with CONDITION)

The dialog allows such commands to be created with the LOCATION keyword being taken as the name of the current object. InForm commands created in this way are held in the Q1 together with the remaining object attributes.


Image: INFORM SOURCES DIALOG - no settings

To create a new InForm command click 'Add InForm'. The dialog will now look like this:


Image: INFORM SOURCES DIALOG - line added

The Keyword and Variable can now be selected from lists. To set the Keyword, click the button in the Keyword column:

   
Image: LIST OF KEYWORDS 

The list of keywords is a sub-set of the full list of InForm commands. Their functions are

If one of the other InForm commands is needed, Go to the Main Menu, InForm Editor and use the traditional InForm format to set the command.

To set the variable, click the box under the 'Var' heading. A list of the variables currently STOREd or SOLVEd will be shown:

Image: LIST OF VARIABLES

Selecting 'New variable' displays a dialog on which the name of the new variable (up to 4 characters long) can be entered. If required, solution of the new variable can also be activated. New variables can also be created from the Main Menu, Models, Solution control / Extra variables panel.

The expression to be used as the 'formula' is entered by clicking on the button under the 'Formula' heading. An editing window will appear, in which the expression can be typed.


Image: INFORM EDITOR

To save the expression and exit click 'File' then 'Save & exit'. In a similar way, any required condition for the expression can be entered into the 'Condition' column. Lines can be up to 1000 characters long. A $ can be freely used as the last character to act as  a continuation-line symbol. When echoed to the Q1, the lines will be folded at column 68 regardless of how they were originally formatted. On the dialog, lines longer than the buttons will be shown as ending in '...'. The full expression will be shown in the editing window.

The 'Del' button will delete the current InForm line. As many InForm commands as required can be added to an object by repeatedly pressing 'Add InForm'.

As an example, the image below shows the settings required to make the inflow mass source and velocity at an INLET a linear function of the Z height.


Image: SETTINGS FOR MASS AND MOMENTUM SOURCES

Lines 1 and 2 set the mass source and momentum source to be linear with ZG, the Z height of the cell centre. The condition on line 1 states that the source is 'per unit area', and the condition on line 2 states that the mass source should be used as a multiplier (see the ONLYMS entry in the Encyclopaedia). Lines 3 and 4 create two local variables for InForm to hold the inlet velocity and density. Finally, lines 5 and 6 set the values for the inlet velocity and density.


Loading a Weather Data File - WIND Object

When 'Use weather data file' is set to Yes, the WIND dialog changes to this:

WIND dialog

IMAGE: WIND Dialog using weather data file

The next task is to select and then configure the data file by clicking Configure file.This leads to a dialog from which the file can be selected and read. The required data items can then be chosen.

Loading a Weather Data File - SUN Object

When 'Use weather data file' is set to Yes, the SUN dialog changes to this:

SUN dialog

IMAGE: WIND Dialog using weather data file

The next task is to select and then configure the data file by clicking Configure file.This leads to a dialog from which the file can be selected and read. The required data items can then be chosen.

Configuring the weather data file - common to WIND and SUN

Configure weather file

IMAGE: Configure weather file

If weather data files in EPW format are already available, they can be selected by clicking NOTSET and browsing to the location of the file. If the required data file is not available, it can be downloaded from the EnergyPlus website by clicking on Start browser. This opens the EnergyPlus site on the page shown here:

Configure weather file

IMAGE: EnergyPlus web site

Choose a region, and then a country within that region. A list of available locations will be shown, for example from the United Kingdom:

Configure weather file

IMAGE: Select location on EnergyPlus web site

The ZIP file for each location contains a number of compressed files. Extract and download the one with the .epw extension, for example GBR_London.gatwick.037760_IWEC.epw. Save it to the current working directory, or any other convenient location. Once the file has been downloaded and saved, it can be attached. This is done by clicking NOTSET next to Weather data file and locating the file in the file browser that opens.

To change the weather file, follow the same procedure. When a weather file has been selected, the dialog shows the name:

Configure weather file

IMAGE: Weather data file selection confirmed

To read the data file, click Load data file. The dialog will update to show the WIND or SUN data that has been read.

Weather data for a WIND object

The dialog will update to show what has been read:

Configure weather file

IMAGE: Weather data for WIND object

The data displayed are for the date and time shown. To select a different month, click the button next to Select month and select from the list. The data will change to that for the same day and time of the new month. To choose a different day and time, click the button next to Using data for, and scroll through the list of available days and times. The data is usually presented on an hourly basis for each day of the month. As shown in the example below, the selection dialog displays the wind direction, speed and air temperature for each entry in the file for the selected month.

Configure weather file

IMAGE: Example selection list for day and time - WIND

Once the date and time have been set, clicking OK on the Configure dialog will return to the Wind Attributes dialog. The data will update to reflect the chosen date and time.

Weather data for a SUN object

The dialog will update to show what has been read:

Configure weather file

IMAGE: Weather data for SUN object

The data displayed are for the date and time shown. To select a different month, click the button next to Select month and select from the list. The data will change to that for the same day and time of the new month. To choose a different day and time, click the button next to Using data for, and scroll through the list of available days and times. The data is usually presented on an hourly basis for each day of the month. As shown in the example below, the selection dialog displays the direct and diffuse solar radiation for each entry in the file for the selected month.

Configure weather file

IMAGE: Example selection list for day and time - SUN

Once the date and time have been set, clicking OK on the Configure dialog will return to the SUN Attributes dialog. The data will update to reflect the chosen date and time.


Contents list