Air conditioning simulation ANSYS Workbench Ott Pabut

Air conditioning simulation ANSYS Workbench 11.00 Ott Pabut Tallinn 2010     Task Set up air conditioning simulation with program Ansys Workbenc...
46 downloads 0 Views 220KB Size
Air conditioning simulation ANSYS Workbench 11.00

Ott Pabut

Tallinn 2010

 

 

Task Set up air conditioning simulation with program Ansys Workbench.

inlet 

heater 

door  windows 

outlet 

thermometer 

Fig1 - Task 1.1 Creating a new project Open program ANSYS Workbench 1. 2. 3. 4.

Click Empty project From the wizard choose File, Save As... Name the project HVAC From the left menu choose Advanced CFD, New Simulation

Workbench offers possibilities for different flow simulations General, Turbomachinery, Quick Setup, Library Template 5. Choose General as the simulation type Now workbench will open the flow simulation preprocessing unit CFX-pre 6. From the wizard choose File, Save Simulation As... Name the project as HVAC.cfx

2   

 

 

1.2 Importing the mesh 1. Choose File, Import mesh... and upload the file named HVACmesh.cfx 2. Save the simulation

1.3 Setting the simulation type 1. Push Simulation Type 2. Apply following settings Tab Basic Settings

Settings Simulation Type > Option Simulation Type > Time Duration > Total Time Simulation Type > Time Steps > Timesteps Simulation Type > Initial Time

Value Transient 45 [s] 3 [s] 0 [s]

3. Push OK

1.4 Creating the computational domain for fluid In the current simulation two different computational domains are created: one for fluid and one for solid (the heater). As the solid and fluid cannot exist in the same space, they must be separated with different domains. 1. On the upper taskbar click Create a Domain 2. Apply the following settings to the domain Tab General options

Fluid Models

Settings Location Basic Settings > Domain Type Basic Settings > Fluids List Domain Models > Pressure > Reference Pressure Domain Models > Buoyancy > Domain Models > Buoyancy > Gravity X Dirn. Domain Models > Buoyancy > Gravity Y Dirn. Domain Models > Buoyancy > Gravity Z Dirn Domain Models > Buoyancy > Bouy. Ref. Density Heat Transfer > Option Thermal Radiation Model > Option 3 

 

and name it FluidZone.

Value B65 Fluid Domain Air Ideal Gas 1 [atm] Buoyant 0 [m/s2] -9.81 [m/s2] 0 [m/s2] 1.2 [kg/m3] Thermal Energy Monte Carlo

 

 

In order to get realistic results the boundary conditions must be similar to those in the reality. Air as an ideal gas is with gravitational force is used and the heat distribution is described with the Monte Carlo statistical method. 3. Click OK

1.5 Creating the computational domain for solid 1. On the upper task bar click Create a Domain 2. Apply the following settings to the domain Tab General options

and name it SolidZone.

Settings Location Basic Settings > Domain Type Basic Settings > Solids List Heat Transfer > Option Thermal Radiation Model Domain Initialization Domain Initialization > Initial Conditions Domain Initialization > Initial Conditions > Temperature > Option Domain Initialization > Initial Conditions > Temperature > Temperature

Solid Models Initialization

Value B18 Solid Domain Copper Thermal Energy Monte Carlo (Selected) (Selected) Automatic with Value 80 [C]

Copper is chosen as the heater material and temperature for the whole volume is 80 C. 3. Click OK 1.6 Inserting the boundary conditions The imported mesh contains predefined 2D regions, which make it easier to apply boundary conditions. For the simulation, following conditions are needed: inlet outlet, windows and walls (no slip condition). Inlet 1. From the upper taskbar click Create a Boundary Condition 2. Name - Inlet (make sure that the domain is FluidZone) 3. Apply following settings Tab Basic Settings

Settings Boundary Type Location

Value Inlet Inlet 4 

 

 

 

Boundary Details

Plot Options

Flow Regime > Option Mass and Momentum > Option Mass and Momentum > Mass Flow Rate Flow Direction > Option Flow Direction > X Component Flow Direction > Y Component Flow Direction > Z Component Heat Transfer > Static Temperature Boundary Vector

Subsonic Mass Flow Rate 0.07 [kg/s] Cartesian Components 5*(x-0.05 [m]) / 1 [m] -1+5*(x-0.05 [m]) / 1 [m] 0 10 [C] (Selected)

Make sure that when describing the flow direction components,the equation writing function is enabled 4. Click OK Outlet 1. Create a new boundary condition Outlet 2. Apply following settings Tab Basic Settings Boundary Details

Settings Boundary Type Location Flow Regime > Option Mass and Momentum > Option Mass and Momentum > Relative Pressure

Value Outlet Outlet Subsonic Average Static Pressure 0 [Pa]

Relative pressure defines the difference between the outlet and inlet pressure, currently the same pressure applies for both and therefore the relative is 0 Pa. 3. Click OK

5   

 

 

Fig 2 – Inlet and Outlet Next the heat flux from the windows is defined Windows 1. Create a new boundary condition Windows 2. Apply the following settings Tab Basic Settings Boundary Details Sources

Settings Boundary Type Location Heat Transfer > Option Heat Transfer > Fixed Temperature Boundary Source Boundary Source > Sources

Value Wall Window1, Window2 Temperature 26 [C] (Selected) (Selected)

3. Create a new radiation source Add New Item and accept the default name 4. Apply the following setting to the Radiation Source. Settings Option Radiation Flux Direction > Option Direction > X Component Direction > Y Component Direction > Z Component 5. Apply the following settings Tab Plot Options

Value Directional Radiation Flux 600 [W/m2] Cartesian Components 0.33 -0.33 -0.33

Settings Boundary Vector

Value (Selected) 6 

 

 

 

6. Click OK Rest of the walls and the door 1. Change the boundary condition FluidZone Default 2. Apply following settings Tab Boundary Details

Settings Heat Transfer > Option Heat Transfer > Fixed Temperature

Value Temperature 26 [C]

3. Click OK 1.7 Setting the initial conditions 1. Click Define the Global Initial Conditions 2. Apply following settings Tab Global Settings

Settings Initial Conditions > Velocity Type Initial Conditions > Cartesian Velocity Components > Options Initial Conditions > Cartesian Velocity Components > U Initial Conditions > Cartesian Velocity Components > V Initial Conditions > Cartesian Velocity Components > W Initial Conditions > Static Pressure > Relative Pressure Initial Conditions > Temperature > Temperature Initial Conditions > Turbulence Kinetic Energy > Fractional Intensity Initial Conditions > Turbulence Eddy Dissipation Initial Conditions > Turbulence Eddy Dissipation > Eddy Length Scale Initial Conditions > Turbulence Eddy Dissipation > Eddy Length Scale > Eddy Len. Scale Initial Conditions > Radiation Intensity > Blackbody Temperature Initial Conditions > Radiation Intensity > Blackbody Temperature > Blackbody Temp.

7   

Value Cartesian Automatic With Value 0 [m s ^-1] 0 [m s ^-1] 0 [m s ^-1] 0 [Pa] 22 [C] (Selected) (Selected) (Selected) 0.25 [m] (Selected) 22 [C]

 

 

3. Click OK 1.8 Modifying the solver control 1. Click Solver Control 2. Apply following settings Tab Basic settings

Settings Transient Scheme > Option Convergence Control > Max. Coeff. Loops

Value Second Order Backward Euler 1

3. Vajuta OK In normal circumstances 3-4 convergence loops are needed to achieve a good result. In this case there are less to save simualting time. 1.9 Setting the output data

1. Click Create Output Files and Monitor Points 2. Click Trn Results 3. Create a new Transient Results unit by clicking Add New Item default name 4. Apply following settings to the Transient Results 1 Settings Option Output Variables List

and accept the

Value Selected Variables Pressure, Radiation Intensity, Temperature, Velocity 3

Output Frequency > Timestep Interval 5. Apply following settings Tab Monitor

Settings Monitor Options

Value (Selected)

6. Create a new Monitor Points and Expressions unit named Thermometer 7. Apply following settings to the Thermometer

Settings Output Variables List Cartesian Coordinates

Value Temperature 3.5, 1.5, 0

8. Click OK

8   

 

 

1.9.1

Getting the result

1. Click Write Solver File 2. Name it HVAC.def 3. Click Save Now Workbench will open Run Definition window 4. Click Start Run Progress of the calculations can be observed form the Momentum and Mass charts. If the results appear to go into the wrong direction, we can stop the calculations and enforce necessary changes. On the right, info about the progress of the calculation and iterations is displayed.

Fig 3 – Progress of the calculations When the number of iterations has been reached or results have converged Workbench will issue a message. To display and process results, question Post-process results now? must be answered “Yes”. To study the simulation progress, the answer should be “No”. The results can also be viewed by selecting CFX-Post form the lower taskbar.

9   

 

 

1.10

Visualization and processing of results

Choose FluidZone and SolidZone in the Domain Selector and click OK. To display results a base plane must be created. 1. From the upper taskbar click Insert, Location, Plane 2. Name it Baseplane 1 3. Apply following settings Tab Geometry

Settings Definition > Method Definition > Z Color Mode Mode > Variable Mode > Range Mode > Min Mode > Max 4. Click Apply

Value XY Plane 1.75 [m] Variable Temperature User Specified 15 [C] 23 [C]

After creating the base plane, temperature on it can be displayed for every time step. 1. Click Timestep Selector 2. Double-click on the step you want to observe Create a second base plane for observing the temperature 1. From the upper taskbar select Insert, Location, Plane 2. Name it Baseplane 2 3. Apply following settings Tab Geometry

Settings Definition > Method Definition > Y Color Mode Mode > Variable Mode > Range Mode > Min Mode > Max 4. Click Apply

Value ZX Plane 0.5 [m] Variable Temperature User Specified 15 [C] 23 [C]

Now isosurface for displaying areas that have the similar temperature is created. 1. Click Insert, Location, Isosurface 2. Name it Isosurface 1 3. Apply following settings 10   

 

 

Tab Geometry Symbol

Settings Definition > Variable Definition > Value Symbol Size

Value Temperature 19 [C] 0.5

4. Click Apply

Fig 3 – Temperature range

11