Chapter 19: Air Conditioning Simulation

This tutorial includes:

Important:  You must have the required Fortran compiler installed and set in your system path in order to run this tutorial. For details on which Fortran compiler is required for your platform, see the applicable Ansys, Inc. installation guide. If you are not sure which Fortran compiler is installed on your system, try running the cfx5mkext command (found in <CFXROOT>/bin) from the command line and read the output messages.

 

19.1. Tutorial Features

In this tutorial you will learn about:

  • Importing CEL expressions.

  • @REGION CEL syntax.

  • Setting up a user CEL function.

  • Setting up a monitor point to observe the temperature at a prescribed location.

  • Setting up an interface with conditional connection control.

  • Using the Monte Carlo radiation model with a directional source of radiation.

  • Postprocessing a transient simulation.

Component

Feature

Details

CFX-Pre

User Mode

General mode

Analysis Type

Transient

Fluid Type

General Fluid

Domain Type

Single Domain

Turbulence Model

k-Epsilon

Heat Transfer

Thermal Energy

Radiation

Monte Carlo

Buoyant Flow

 

Boundary Conditions

Boundary Profile Visualization

Inlet (Profile)

Outlet (Subsonic)

Wall: No-Slip

Wall: Adiabatic

Wall: Fixed Temperature

Domain Interface

Conditional GGI

Output Control

Transient Results Files

Monitor Points

CEL (CFX Expression Language)

User CEL Function

CFD-Post

Plots

Animation

Isosurface

Point

Slice Plane

Other

Text Label with Auto Annotation

Changing the Color Range

Legend

Time Step Selection

Transient Animation with Movie Generation

 

19.2. Overview of the Problem to Solve

This tutorial simulates a room with a thermostat-controlled air conditioner adjacent to a closet. The closet door is initially closed and opens during the simulation.

The thermostat switches the air conditioner on and off based on the following data:

  • A set point of 22°C (the temperature at or above which the air conditioner turns on)

  • A temperature tolerance of 1°C (the amount by which cooling continues below the set point before the air conditioner turns off)

  • The temperature at a wall-mounted thermometer

Air flows in steadily from an inlet vent on the ceiling, and flows out through a return-air vent near the floor. When the air conditioner is turned on, the incoming air temperature is reduced compared to the outgoing air temperature. When the air conditioner is turned off, the incoming air temperature is set equal to the outgoing air temperature.

Two windows enable sunlight to enter and heat the room. The walls (except for the closet door and part of the wall surrounding the closet door) and windows are assumed to be at a constant 26 °C. The simulation is transient, and continues long enough to enable the air conditioner to cycle on and off.

If this is the first tutorial you are working with, it is important to review the following topics before beginning:

 

19.3. Preparing the Working Directory

  1. Create a working directory.

    Ansys CFX uses a working directory as the default location for loading and saving files for a particular session or project.

  2. Download the hvac.zip file here .

  3. Unzip hvac.zip to your working directory.

    Ensure that the following tutorial input files are in your working directory:

    • HVAC_expressions.ccl

    • HVACMesh.gtm

    • TStat_Control.F

      Note:  You must have a Fortran compiler installed on your system to perform this tutorial.

  4. Set the working directory and start CFX-Pre.

    For details, see Setting the Working Directory and Starting Ansys CFX in Stand-alone Mode.

 

19.4. Defining the Case Using CFX-Pre

  1. In CFX-Pre, select File > New Case.

  2. Select General and click OK.

  3. Select File > Save Case As.

  4. Under File name, type HVAC.

  5. Click Save.

 

19.4.1. Importing the Mesh

  1. Right-click Mesh and select Import Mesh > CFX Mesh.

    The Import Mesh dialog box appears.

  2. Configure the following setting(s):

    Setting

    Value

    File name

    HVACMesh.gtm

  3. Click Open.

  4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up) from the shortcut menu.

 

19.4.2. Importing CEL Expressions

This tutorial uses several CEL expressions to store parameters and to evaluate other quantities that are required by the simulation. Import all of the expressions from the provided file:

  1. Select File > Import > CCL.

  2. Ensure that Import Method is set to Append.

  3. Select HVAC_expressions.ccl, which should be in your working directory.

  4. Click Open.

The table below lists the expressions, along with the definition and information for each expression:

Expression Name

Expression Definition

Information

ACOn

Thermostat Function(TSensor,TSet,TTol,atstep)

On/off status of the air conditioner (determined by calling a user CEL function with the thermometer temperature, thermostat set point, and temperature tolerance).

Cool TempCalc

TVentOut - (HeatRemoved / (MassFlow * 1.004 [kJ kg^-1 K^-1 ]))

Temperature of air at the return-air vent (determined by a CEL function).

Flowrate

0.06 [m^3 s^-1]

Volumetric flow rate of air entering the room.

HeatRemoved

1000 [J s^-1]

Rate of thermal energy removal when the air conditioner is on.

MassFlow

1.185 [kg m^-3] * Flowrate

Mass flow rate of air entering the room.

TIn

ACOn*CoolTempCalc+(1-ACOn)*TVentOut

Temperature of inlet vent air (a function of the air conditioner on/off status, return-air vent temperature, thermal energy removal rate, and mass flow rate).

TSensor

probe(T)@Thermometer

Thermometer temperature (determined by a CEL function that gets temperature data from a monitor point).

TSet

22 [C]

Thermometer set point.

TTol

1 [K]

Temperature tolerance.

TVentOut

areaAve(T)@REGION:VentOut

Temperature of outlet vent air.

XCompInlet

5*(x-0.05 [m]) / 1 [m]

Direction vector components for guiding the inlet vent air in a diverging manner as it enters the room.

ZCompInlet

-1+XCompInlet

tStep

3 [s]

Time step size.

tTotal

225 [s]

Total time.

The CEL function that evaluates the thermometer temperature relies on a monitor point that you will create later in this tutorial.

The CEL expression for the air conditioner on/off status requires a compiled Fortran subroutine and a user CEL function that uses the subroutine. These are created next, starting with the compiled subroutine.

Note:  The expression for the return-air vent temperature, TVentOut, makes use of @REGION CEL syntax, which indicates the mesh region named VentOut, rather than a boundary named VentOut.

 

19.4.3. Compiling the Fortran Subroutine for the Thermostat

A Fortran subroutine that simulates the thermostat is provided with the tutorial input files. Before the subroutine can be used, it must be compiled for your platform.

You can compile the subroutine at any time before running CFX-Solver. The operation is performed at this point in the tutorial so that you have a better understanding of the values you need to specify in CFX-Pre when creating a User CEL Function. The cfx5mkext command is used to compile the subroutine as described below.

  1. Ensure that file TStat_Control.F is in your working directory.

    You can examine the contents of this file in any text editor to gain a better understanding of the subroutine it contains.

  2. Select Tools > Command Editor.

  3. Type the following command in the Command Editor dialog box (make sure you do not miss the semicolon at the end of the line):

    ! system ("cfx5mkext TStat_Control.F") == 0 or die "cfx5mkext failed";

    • This is equivalent to executing the following at a command prompt:

      cfx5mkext TStat_Control.F

    • The ! indicates that the following line is to be interpreted as power syntax and not CCL. Everything after the ! symbol is processed as Perl commands.

    • system is a Perl function to run a system command.

    • The "== 0 or die" will cause an error message to be returned if, for some reason, there is an error in processing the command.

  4. Click Process to compile the subroutine.

    Note:  You can use the -double option to compile the subroutine for use with double precision CFX-Solver executables. That is:

    cfx5mkext -double TStat_Control.F

A subdirectory will have been created in your working directory whose name is system dependent (for example, on Linux it is named linux). This subdirectory contains the shared object library.

Note:  If you are running problems in parallel over multiple platforms then you will need to create these subdirectories using the cfx5mkext command for each different platform.

  • You can view more details about the cfx5mkext command by running:

    cfx5mkext -help

  • You can set a Library Name and Library Path using the -name and -dest options respectively.

  • If these are not specified, the default Library Name is that of your Fortran file and the default Library Path is your current working directory.

  • Close the Command Editor dialog box.

 

19.4.4. Creating a User CEL Function for the Thermostat

The expression for the air conditioner on/off status is named ACOn. This expression consists of a call to a user CEL function, Thermostat Function, which must be created.

Before you create the user CEL function, you will first create a user routine that holds basic information about the compiled Fortran subroutine. You will then create a user function, Thermostat Function, so that it is associated with the user routine.

Create the user routine:

  1. From the main menu, select Insert > Expressions, Functions and Variables > User Routine or click User Routine  .

  2. Set the name to Thermostat Routine.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Option

    User CEL Function

    Calling Name

    		ac_on [a]

    Library Name

    TStat_Control [b]

    Library Path

    (Working Directory) [c]

    1. This is the name of the subroutine within the Fortran file. Always use lower case letters for the calling name, even if the subroutine name in the Fortran file is in upper case.

    2. This is the name passed to the cfx5mkext command by the -name option. If the -name option is not specified, a default is used. The default is the Fortran file name without the .F extension.

    3. Set this to your working directory.

  4. Click OK.

Create the user CEL function:

  1. From the main menu, select Insert > Expressions, Functions and Variables > User Function or click User Function  .

  2. Set the name to Thermostat Function.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Option

    User Function

    User Routine Name

    Thermostat Routine

    Argument Units

    [K], [K], [K], [] [a]

    Result Units

    [] [b]

    1. These are the units for the four input arguments: TSensor, TSet, TTol, and atstep.

    2. The result will be a dimensionless flag with a value of 0 or 1.

  4. Click OK.

 

19.4.5. Setting the Analysis Type

This is a transient simulation. The total time and time step are specified by expressions that you imported earlier. Use these expressions to set up the Analysis Type information:

  1. Right-click Analysis Type in the Outline tree view and select Edit.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Analysis Type

    > Option

     

    Transient

    Analysis Type

    > Time Duration

    > Option

     

     

    Total Time

    Analysis Type

    > Time Duration

    > Total Time

     

     

    tTotal

    Analysis Type

    > Time Steps

    > Option

     

     

    Timesteps

    Analysis Type

    > Time Steps

    > Timesteps

     

     

    tStep

    Analysis Type

    > Initial Time

    > Option

     

     

    Automatic with Value

    Analysis Type

    > Initial Time

    > Time

     

     

    0 [s]

  3. Click OK.

 

19.4.6. Creating the Domain

The domain that models the room air should model buoyancy, given the expected temperature differences, air speeds, and the size and geometry of the room. The domain must model radiation, since directional radiation (representing sunlight) will be emitted from the windows.

Create the domain:

  1. Edit Case Options > General in the Outline tree view and ensure that Automatic Default Domain is turned on.

    A domain named Default Domain should appear under the Simulation branch.

  2. Edit Default Domain and configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Location and Type

    > Location

     

    B54,B64

    Fluid and Particle Definitions

    Fluid 1

    Fluid and Particle Definitions

    > Fluid 1

    > Material

     

     

    Air Ideal Gas

    Domain Models

    > Pressure

    > Reference Pressure

     

     

    1 [atm]

    Domain Models

    > Buoyancy Model

    > Option

     

     

    Buoyant

    Domain Models

    > Buoyancy Model

    > Gravity X Dirn.

     

     

    0 [m s^-2]

    Domain Models

    > Buoyancy Model

    > Gravity Y Dirn.

     

     

    0 [m s^-2]

    Domain Models

    > Buoyancy Model

    > Gravity Z Dirn.

     

     

    -g

    Domain Models

    > Buoyancy Model

    > Buoy. Ref. Density

     

     

    1.2 [kg m^-3]

    Fluid Models

    Heat Transfer

    > Option

     

    Thermal Energy

    Turbulence

    > Option

     

    k-Epsilon

    Thermal Radiation

    > Option

     

    Monte Carlo

    Thermal Radiation

    > Number of Histories

     

    100000

  3. Click OK.

Note:  When using a statistical radiation model like Monte Carlo, the results can usually be improved (at the expense of increased computational time) by increasing the number of histories.

 

19.4.7. Creating the Boundaries

In this section you will define several boundaries:

  • An inlet vent that injects air into the room.

  • A return-air vent that lets air leave the room.

  • Fixed-temperature windows that emit directed radiation.

  • Fixed-temperature walls.

 

19.4.7.1. Inlet Boundary

Create a boundary for the inlet vent, using the previously-loaded expressions for mass flow rate, flow direction, and temperature:

  1. Create a boundary named Inlet.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Inlet

    Location

    Inlet

    Boundary Details

    Mass and Momentum

    > Option

     

    Mass Flow Rate

    Mass and Momentum

    > Mass Flow Rate

     

    MassFlow

    Flow Direction

    > Option

     

    Cartesian Components

    Flow Direction

    > X Component

     

    XCompInlet

    Flow Direction

    > Y Component

     

    0

    Flow Direction

    > Z Component

     

    ZCompInlet

    Heat Transfer

    > Option

     

    Static Temperature

    Heat Transfer

    > Static Temperature

     

    TIn

    Plot Options

    Boundary Vector

    (Selected)

    Boundary Vector

    > Profile Vec. Comps.

     

    Cartesian Components

  3. Click OK.

    The viewer shows the inlet velocity profile applied at the inlet, which uses the expressions XCompInlet and ZCompInlet to specify a diverging flow pattern.

    Note:  Ignore the physics errors that appear. They will be fixed by setting up the rest of the simulation. The error concerning the expression TIn is due to a reference to Thermometer, which does not yet exist. A monitor point named Thermometer will be created later as part of the output control settings.

 

19.4.7.2. Outlet Boundary

Create a boundary for the return-air vent, specifying a relative pressure of 0 Pa:

  1. Create a boundary named VentOut.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Outlet

    Location

    VentOut

    Boundary Details

    Mass and Momentum

    > Option

     

    Average Static Pressure

    Mass and Momentum

    > Relative Pressure

     

    0 [Pa]

  3. Click OK.

 

19.4.7.3. Window Boundary

To model sunlight entering the room, the windows are required to emit directional radiation. To approximate the effect of the outdoor air temperature, assume that the windows have a fixed temperature of 26°C.

Create a boundary for the windows using a fixed temperature of 26°C and apply a radiation source of 600 W m^-2 in the (1, 1, -1) direction:

  1. Create a boundary named Windows.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Wall

    Location

    Window1,Window2

    Boundary Details

    Heat Transfer

    > Option

     

    Temperature

    Heat Transfer

    > Fixed Temperature

     

    26 [C]

    Sources

    Boundary Source

    (Selected)

    Boundary Source

    > Sources

     

    (Selected)

  3. Create a new radiation source item by clicking Add new item   and accepting the default name.

  4. Configure the following setting(s) of Radiation Source 1:

    Setting

    Value

    Option

    Directional Radiation Flux

    Radiation Flux

    600 [W m^-2]

    Direction

    > Option

     

    Cartesian Components

    Direction

    > X Component

     

    1

    Direction

    > Y Component

     

    1

    Direction

    > Z Component

     

    -1

  5. Configure the following setting(s):

    Tab

    Setting

    Value

    Plot Options

    Boundary Vector

    (Selected)

    Boundary Vector

    > Profile Vec. Comps.

     

    Cartesian Components in Radiation Source 1

  6. Click OK.

    The direction of the radiation is shown in the viewer.

 

19.4.7.4. Default Wall Boundary

The default boundary for any undefined surface in CFX-Pre is a no-slip, smooth, adiabatic wall. For this simulation, assume that the walls have a fixed temperature of 26°C. A more detailed simulation would model heat transfer through the walls.

For radiation purposes, assume that the default wall is a perfectly absorbing and emitting surface (emissivity = 1).

Set up the default wall boundary:

  1. Edit the boundary named Default Domain Default.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Boundary Details

    Heat Transfer

    > Option

     

    Temperature

    Heat Transfer

    > Fixed Temperature

     

    26 [C]

    Thermal Radiation

    > Option

     

    Opaque

    Thermal Radiation

    > Emissivity

     

    1

  3. Click OK.

Because this boundary is opaque with an emissivity of 1, all of the radiation is absorbed and none of the radiation is reflected. With no reflected radiation, the Diffuse Fraction setting has no effect. For lower values of emissivity, some radiation is reflected, and the Diffuse Fraction setting controls the fraction of the reflected radiation that is diffuse, with the remainder being specular (directional).

 

19.4.8. Closet Wall Interface

  1. Click Domain Interface  , set Name to ClosetWall, and click OK.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Interface Side 1

    > Region List

     

    F51.54

    Interface Side 2

    > Region List

     

    F51.64

    Additional Interface Models

    Mass And Momentum

    > Option

    No Slip Wall

    Heat Transfer

    (Selected)

    Heat Transfer

    > Option

     

    Conservative Interface Flux

    Heat Transfer

    > Interface Model

    > Option

     

     

    Thin Material

    Heat Transfer

    > Interface Model

    > Material

     

     

    Building Board Hardwood [a]

    Heat Transfer

    > Interface Model

    > Thickness

     

     

    12 [cm]

    Thermal Radiation

    (Selected)

    Thermal Radiation

    > Option

     

    Opaque

    Thermal Radiation

    > Emissivity

     

    1

    1. Click the Ellipsis   icon to open the Material dialog box. Click Import Library Data  . In the Select Library Data to Import dialog box, select Building Board Hardwood under the CHT Solids branch and click OK. In the Material dialog box, select Building Board Hardwood under the CHT Solids branch and click OK.

  3. Click OK.

 

19.4.9. Creating a Logical Expression for the Conditional GGI Interface

Create an expression named tOpen:

  1. In the Outline tree view, expand Expressions, Functions and Variables, right-click Expressions and select Insert > Expression

  2. Give the new expression the name: tOpen

  3. In the Definition area, type t>150[s].

  4. Click Apply.

This expression will be used to indicate the point at which the closet door is to open during the simulation. In the next section, you will set up the door interface, and indicate that the interface should change from closed to open when the expression tOpen evaluates to 1[] (true).

 

19.4.10. Creating a Conditional GGI Interface for the Closet Door

Create the interface:

  1. Click Domain Interface  , set Name to ClosetDoor, and click OK.

  2. Configure the following settings:

    Tab

    Setting

    Value

    Basic Settings

    Interface Side 1

    > Region List

     

    F53.54

    Interface Side 2

    > Region List

     

    F53.64

    Additional Interface Models

    Mass And Momentum

    > Option

     

    Conservative Interface Flux

    Conditional Connection Control

    (Selected)

    Conditional Connection Control

    > Option

     

    Irreversible State Change

    Conditional Connection Control

    > Logical Expression

     

    tOpen

    Conditional Connection Control

    > Initial State

     

    Closed

  3. Click OK.

Next, set the properties of the closet door that will apply when the door is closed:

  1. Edit the boundary named ClosetDoor Side 1.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Nonoverlap Conditions

    Nonoverlap Conditions

    (Selected)

    Nonoverlap Conditions

    > Boundary Type

     

    Wall

    Nonoverlap Conditions

    > Mass and Momentum

    > Option

     

     

    No Slip Wall

    Nonoverlap Conditions

    > Heat Transfer

    > Option

     

     

    Adiabatic

    Nonoverlap Conditions

    > Thermal Radiation

    > Option

     

     

    Opaque

    Nonoverlap Conditions

    > Thermal Radiation

    > Emissivity

     

     

    1

  3. Click OK.

  4. Do the same for ClosetDoor Side 2.

 

19.4.11. Creating Space Under the Closet Door

Create an interface under the closet door so that air can pass freely under the door. This connection will prevent the air in the closet from becoming isolated, so that the pressure level in the closet will be constrained.

  1. Click Domain Interface  , set Name to DoorSpace, and click OK.

  2. Configure the following settings:

    Tab

    Setting

    Value

    Basic Settings

    Interface Side 1

    > Region List

     

    F52.54

    Interface Side 2

    > Region List

     

    F52.64

  3. Click OK.

 

19.4.12. Setting Initial Values

  1. Click Global Initialization  .

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Global Settings

    Initial Conditions

    > Velocity Type

     

    Cartesian

    Initial Conditions

    > Cartesian Velocity Components

    > Option

     

     

    Automatic with Value

    Initial Conditions

    > Cartesian Velocity Components

    > U

     

     

    0 [m s^-1]

    Initial Conditions

    > Cartesian Velocity Components

    > V

     

     

    0 [m s^-1]

    Initial Conditions

    > Cartesian Velocity Components

    > W

     

     

    0 [m s^-1]

    Initial Conditions

    > Static Pressure

    > Option

     

     

    Automatic with Value

    Initial Conditions

    > Static Pressure

    > Relative Pressure

     

     

    0 [Pa]

    Initial Conditions

    > Temperature

    > Option

     

     

    Automatic with Value

    Initial Conditions

    > Temperature

    > Temperature

     

     

    21.8 [C]

    Initial Conditions

    > Turbulence

    > Option

     

     

    Intensity and Length Scale

    Initial Conditions

    > Turbulence

    > Fractional Intensity

    > Option

     

     

     

    Automatic with Value

    Initial Conditions

    > Turbulence

    > Fractional Intensity

    > Value

     

     

     

    0.05

    Initial Conditions

    > Turbulence

    > Eddy Length Scale

    > Option

     

     

     

    Automatic with Value

    Initial Conditions

    > Turbulence

    > Eddy Length Scale

    > Value

     

     

     

    0.25 [m]

    Initial Conditions

    > Radiation Intensity

    > Option

     

     

    Automatic with Value

    Initial Conditions

    > Radiation Intensity

    > Blackbody Temperature

     

     

    (Selected)

    Initial Conditions

    > Radiation Intensity

    > Blackbody Temperature

    > Blackbody Temp.

     

     

     

    21.8 [C] [a]

    1. The initial blackbody temperature of the air should be set to the initial temperature of the air.

  3. Click OK.

 

19.4.13. Setting Solver Control

In a typical transient simulation, there should be sufficient coefficient loops per time step to achieve convergence. In order to reduce the time required to run this particular simulation, reduce the maximum number of coefficient loops per time step to 3:

  1. Click Solver Control  .

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Convergence Control

    > Max. Coeff. Loops

     

    3

  3. Click OK.

 

19.4.14. Setting Output Control

Set up the solver to output transient results files that record pressure, radiation intensity, temperature, and velocity, on every time step:

  1. Click Output Control  .

  2. Click the Trn Results tab.

  3. In the Transient Results list box, click Add new item  , set Name to Transient Results 1, and click OK.

  4. Configure the following setting(s) of Transient Results 1:

    Setting

    Value

    Option

    Selected Variables

    Output Variables List

    Pressure, Radiation Intensity, Temperature, Velocity [a]

    Output Variable Operators

    (Selected)

    Output Variable Operators

    > Output Variable Operators

     

    All [b]

    Output Frequency

    > Option

     

    Every Timestep

    1. Use the Ctrl key to select more than one variable.

    2. This causes the gradients of the selected variables to be written to the transient results files, along with other information.

To create the thermostat thermometer, set up a monitor point at the thermometer location. Also set up monitors to track the expressions for the temperature at the inlet, the temperature at the outlet, and the on/off status of the air conditioner.

  1. Configure the following setting(s):

    Tab

    Setting

    Value

    Monitor

    Monitor Objects

    (Selected)

  2. Create a new Monitor Points and Expressions item named Thermometer.

  3. Configure the following setting(s) of Thermometer:

    Setting

    Value

    Output Variables List

    Temperature

    Cartesian Coordinates

    2.95, 1.5, 1.25

  4. Create a new Monitor Points and Expressions item named Temp at Inlet.

  5. Configure the following setting(s) of Temp at Inlet:

    Setting

    Value

    Option

    Expression

    Expression Value

    TIn

  6. Create a new Monitor Points and Expressions item named Temp at VentOut.

  7. Configure the following setting(s) of Temp at VentOut:

    Setting

    Value

    Option

    Expression

    Expression Value

    TVentOut

  8. Create a new Monitor Points and Expressions item named ACOnStatus.

  9. Configure the following setting(s) of ACOnStatus:

    Setting

    Value

    Option

    Expression

    Expression Value

    ACOn

  10. Click OK.

 

19.4.15. Writing the CFX-Solver Input (.def) File

  1. Click Define Run  .

  2. Configure the following setting(s):

    Setting

    Value

    File name

    HVAC.def

  3. Click Save.

    CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

  4. If using stand-alone mode, quit CFX-Pre, saving the simulation (.cfx) file at your discretion.

 

19.5. Obtaining the Solution Using CFX-Solver Manager

When CFX-Pre has shut down and CFX-Solver Manager has started, start the solver and view the monitor points as the solution progresses:

  1. Click Start Run.

    After a few minutes, a User Points tab will appear.

    On that tab, plots will appear showing the values of the monitor points:

    • ACOnStatus

    • Temp at Inlet

    • Temp at VentOut

    • Thermometer (Temperature)

  2. Click one of the plot lines to see the value of the plot variable at that point.

  3. It is difficult to see the plot values because all of the monitor points are plotted on the same scale. To see the plots in more detail, try displaying subsets of them as follows:

    1. Right-click in the plot area and select Monitor Properties from the shortcut menu.

    2. In the Monitor Properties dialog box, on the Plot Lines tab, expand the USER POINT branch in the tree.

    3. Clear the check boxes beside all of the monitor points except ACOnStatus, then click Apply.

    4. Observe the plot for ACOnStatus.

      You might have to move the dialog box out of the way to see the plot.

    5. In the Monitor Properties dialog box, toggle each of the check boxes beside the monitor points, so that all of the monitor points are selected except for ACOnStatus, then click Apply.

    6. Observe the plots for Temp at Inlet, Temp at VentOut, and Thermometer (Temperature).

    7. Click OK to close the Monitor Properties dialog box.

  4. Select the check box next to Post-Process Results when the completion message appears at the end of the run.

  5. If using stand-alone mode, select the check box next to Shut down CFX-Solver Manager.

  6. Click OK.

 

19.6. Viewing the Results Using CFD-Post

You will first create some graphic objects to visualize the temperature distribution and the thermometer location. You will then create an animation to show how the temperature distribution changes.

 

19.6.1. Creating Graphics Objects

In this section, you will create two planes and an isosurface of constant temperature, all colored by temperature. You will also create a color legend and a text label that reports the thermometer temperature.

 

19.6.1.1. Creating Planes

In order to show the key features of the temperature distribution, create two planes colored by temperature as follows:

  1. Load the res file (HVAC_001.res) if you did not elect to load the results directly from CFX-Solver Manager.

  2. Right-click a blank area in the viewer, select Predefined Camera > Isometric View (Z up).

  3. Create a ZX-Plane named Plane 1 with Y=2.25 [m]. Color it by Temperature using a user specified range from 19 [C] to 23 [C]. Turn off lighting (on the Render tab) so that the colors are accurate and can be interpreted properly using the legend.

  4. Create an XY plane named Plane 2 with Z=0.35 [m]. Color it using the same settings as for the first plane, and turn off lighting.

 

19.6.1.2. Creating an Isosurface

In order to show the plumes of cool air from the inlet vent, create a surface of constant temperature as follows:

  1. Click Timestep Selector  . The Timestep Selector dialog box appears.

  2. Double-click the value: 69 s.

    The time step is set to 69 s so that the cold air plume is visible.

  3. Create an isosurface named Cold Plume as a surface of Temperature = 19 °C.

  4. Color the isosurface by Temperature (select Use Plot Variable) and use the same color range as for the planes. Although the color of the isosurface will not show variation (by definition), it will be consistent with the coloration of the planes.

  5. On the Render tab for the isosurface, set Transparency to 0.5. Leave lighting turned on to help show the 3D shape of the isosurface.

  6. Click Apply.

    Note:  The isosurface will not be visible in some time steps, but you will be able to see it when playing the animation (a step carried out later).

 

19.6.1.3. Adjusting the Legend

The legend title should not name the locator of any particular object since all objects are colored by the same variable and use the same range. Remove the locator name from the title and, in preparation for making an MPEG video later in this tutorial, increase the text size:

  1. Edit Default Legend View 1.

  2. On the Definition tab, change Title Mode to Variable.

    This will remove the locator name from the legend.

  3. Click the Appearance tab, then:

    1. Change Precision to 2, Fixed.

    2. Change Text Height to 0.03.

  4. Click Apply.

 

19.6.1.4. Creating a Point for the Thermometer

In the next section, you will create a text label that displays the value of the expression TSensor, which represents the thermometer temperature. During the solver run, this expression was evaluated using a monitor point named Thermometer. Although this monitor point data is stored in the results file, it cannot be accessed. In order to support the expression for TSensor, create a point called Thermometer at the same location:

  1. From the main menu, select Insert > Location > Point.

  2. Set Name to Thermometer.

  3. Set Point to (2.95,1.5,1.25).

  4. Click the Color tab, then change Color to blue.

  5. Click Apply.

    A marker appears at the thermometer location in the viewer. Note that you may have to rotate the results data to see the point.

 

19.6.1.5. Creating a Text Label

Create a text label that shows the currently-selected time step and thermometer temperature.

  1. Click Text  .

  2. Accept the default name and click OK.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Definition

    Text String

    Time Elapsed:

    Embed Auto Annotation

    (Selected) [a]

    Type

    Time Value

    1. The full text string should now be Time Elapsed: <aa>. The <aa> string represents the location where text is to be substituted.

  4. Click More to add a second line of text to the text object.

  5. Configure the following setting(s):

    Tab

    Setting

    Value

    Definition

    Text String (the second one)

    Sensor Temperature:

    Embed Auto Annotation

    (Selected)

    Type

    Expression

    Expression

    TSensor

    Appearance

    Height

    0.03

  6. Click Apply.

  7. Ensure that the visibility for Text 1 is turned on.

The text label appears in the viewer, near the top.

 

19.6.2. Creating an Animation

  1. Ensure that the view is set to Isometric View (Z up).

  2. Click Timestep Selector  .

  3. Double-click the first time value (0 s).

  4. Click Animation  .

    The Animation dialog box appears.

  5. Set Type to Keyframe Animation.

  6. Click New   to create KeyframeNo1.

  7. Select KeyframeNo1, then set # of Frames to 200, then press Enter while in the # of Frames box.

    Tip:  Be sure to press Enter and confirm that the new number appears in the list before continuing.

    This will place 200 intermediate frames between the first and (yet to be created) second key frames, for a total of 202 frames. This will produce an animation lasting about 8.4 s since the frame rate will be 24 frames per second. Since there are 76 unique frames, each frame will be shown at least once.

  8. Use the Timestep Selector to load the last time value (225 s).

  9. In the Animation dialog box, click New   to create KeyframeNo2.

    The # of Frames parameter has no effect for the last keyframe, so leave it at the default value.

  10. Click More Animation Options   to expand the Animation dialog box.

  11. Select Save Movie.

  12. Set Format to MPEG1.

  13. Specify a filename for the movie.

  14. Click the Options button.

  15. Change Image Size to 720 x 480 (or a similar resolution).

  16. Click the Advanced tab, and note the Quality setting. If your movie player cannot play the resulting MPEG, you can try using the Low or Custom quality settings.

  17. Click OK.

  18. Click To Beginning   to rewind the active key frame to KeyframeNo1.

  19. Click Save animation state   and save the animation to a file. This will enable you to quickly restore the animation in case you want to make changes. Animations are not restored by loading ordinary state files (those with the .cst extension).

  20. Click Play the animation  .

  21. If prompted to overwrite an existing movie, click Overwrite.

    The animation plays and builds an mpg file.

  22. When you have finished, quit CFD-Post.

 

19.7. Further Discussion

  • This tutorial uses an aggressive flow rate of air, a coarse mesh, large time steps, and a low cap on the maximum number of coefficient loops per time step. Running this tutorial with a flow rate of air that is closer to 5 changes of air per hour (0.03 m3 s-1), a finer mesh, smaller time steps, and a larger cap on the maximum number of coefficient loops, will produce more accurate results.

  • Running this simulation for a longer total time will allow you to see more on/off cycles of the air conditioner.