Introduction to CFX. Workshop 3 Room Temperature Study

1. Workshop 3 Room Temperature Study

Introduction to CFX
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-1
April 28, 2009
Inventory #002599

2. Introduction

WS3: Room Temperature Study
Introduction
Workshop Supplement
In this workshop you will be analyzing the effect of computers and
workers on the temperature distribution in an office. In the first stage
airflow through the supply air ducts will be simulated and the outlet
conditions for the duct will be used to set the inlet conditions for the
room. Although both components could be analyzed together,
separating the two components allows different room configurations to
be analyzed without solving the duct flow again.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-2
April 28, 2009
Inventory #002599

3. Duct Simulation

WS3: Room Temperature Study
Duct Simulation
Workshop Supplement
• The operating conditions for the flow are:
The working fluid is Air Ideal Gas
Fluid Temperature = 21 [C]
Inlet: 0 [atm] Total Pressure
Outlet: 0.225 [kg/s] (per vent)
vent2
Inlet
vent1
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-3
April 28, 2009
Inventory #002599

4. Starting CFX in Workbench

WS3: Room Temperature Study
Starting CFX in Workbench
Workshop Supplement
1. Open Workbench
2. Drag CFX into the Project Schematic from the Component Systems
toolbox
3. Change the name of the system to duct
4. Save the project as RoomStudy.wbpj in an appropriate directory
5. Double-click Setup
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-4
April 28, 2009
Inventory #002599

5. Import Mesh

WS3: Room Temperature Study
Import Mesh
Workshop Supplement
The first step is to import the mesh that has already been created:
1. Right-click on Mesh in the Outline tree and select Import Mesh > ICEM
CFD
2. Select the file duct_mesh.cfx5
3. Make sure Mesh Units are in m and click Open to import the mesh
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-5
April 28, 2009
Inventory #002599

6. Create Domain

WS3: Room Temperature Study
Create Domain
Workshop Supplement
You can now create the computational domain:
1. Double-click on Default Domain in the Outline tree to edit the domain
2. On the Basic Settings tab, set the Fluid 1 Material setting to Air Ideal
Gas
3. Switch to the Fluid Models tab
4. Set the Heat Transfer Option to Isothermal
–
Heat Transfer is not modeled, but since the working fluid is an ideal gas
we need to provide a temperature so its properties can be calculated
5. Set the Fluid Temperature to 21 [C]
6. Change the Turbulence Model Option to Shear Stress Transport
7. Click OK to commit the changes to the domain
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-6
April 28, 2009
Inventory #002599

7. Create Boundary Conditions

WS3: Room Temperature Study
Create Boundary Conditions
Workshop Supplement
Now create the following boundary conditions:
1. INLET Boundary Condition
2. VENT1 Boundary Condition
–
–
–
–
–
–
–
–
Name: VENT1
Boundary Type: Outlet
Location: VENT1
Mass and Momentum Option:
Mass Flow Rate
– Mass Flow Rate: 0.225 [kg/s]
Name: INLET
Boundary Type: Inlet
Location: INLET
Mass and Momentum Option:
Total Pressure (stable)
– Relative Pressure: 0 [Pa]
3. VENT2 Boundary Condition
–
–
–
–
Name: VENT2
Boundary Type: Outlet
Location: VENT2
Mass and Momentum Option:
Mass Flow Rate
– Mass Flow Rate: 0.225 [kg/s]
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-7
April 28, 2009
Inventory #002599

8. Solver Control

WS3: Room Temperature Study
Solver Control
Workshop Supplement
1. Double click on Solver Control from the Outline tree
2. Enable the Conservation Target toggle
The default Conservation Target is 1%. This means that the
global imbalance for each equation must be less than 1% (i.e.
(flux in – flux out)/flux in < 1%). The solver will not stop until
both the Residual Target and the Conservation Target have
been met (or Max. Iterations is reached).
3. Click OK to commit the settings
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-8
April 28, 2009
Inventory #002599

9. Monitor Point

WS3: Room Temperature Study
Monitor Point
Workshop Supplement
Monitor points are used to monitor quantities of interest during the
solution. They should be used to help judge convergence. In this case
you will monitor the velocity of the air that exits through the vent. One
measure of a converged solution is when this air has reached a steadystate velocity.
1.
2.
3.
4.
5.
Double click on Output Control from the Outline tree
Switch to the Monitor tab and enable the Monitor Options toggle
Under Monitor Points and Expressions, click the New icon
Keep the default name Monitor Point 1
Set the Option to Expression
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-9
April 28, 2009
Inventory #002599

10. Monitor Point

WS3: Room Temperature Study
Monitor Point
Workshop Supplement
6. In the Expression Value field, type in:
areaAve(Velocity w)@VENT1
7. Click OK to create the Monitor Point
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-10
April 28, 2009
Inventory #002599

11. Write Solver File

WS3: Room Temperature Study
Write Solver File
Workshop Supplement
You can now save the project and proceed to write a definition file for
the solver:
1.
2.
3.
4.
Close CFX-Pre to return to Project window
Save the project
Right-click on Solution and select Edit
Choose Start Run
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-11
April 28, 2009
Inventory #002599

12. CFX Solver Manager

WS3: Room Temperature Study
CFX Solver Manager
Workshop Supplement
1. Examine the residual plots for Momentum and Mass and Turbulence
2. Examine the User Points plot
Monitor point
Residual plot
3. When the run finished close the Solver Manager
4. View the results in CFD-Post by double-clicking Results in the Project
window
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-12
April 28, 2009
Inventory #002599

13. CFD-Post

WS3: Room Temperature Study
CFD-Post
Workshop Supplement
Now we will export a Boundary Condition profile from the outlet regions for
use in the next simulation.
1. Select File > Export
2. Change the file name to vent1.csv
3. Use the browse icon to set an appropriate
directory
4. Set Type as BC Profile and Locations as
VENT1
5. Leave Profile Type as Inlet Velocity and
click Save
6. Similarly export a BC profile of VENT2 to
the file named vent2.csv
7. Quit CFD-Post and return to the Project
Schematic
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-13
April 28, 2009
Inventory #002599

14. Operating Conditions

WS3: Room Temperature Study
Operating Conditions
Workshop Supplement
The operating conditions for the flow in the room are:
The working fluid is Air Ideal Gas
Computer Monitor Temperature = 30 [C]
Computer Vent Flow Rate: 0.033 [kg/s] @ 40 [C] (per computer)
Ceiling Vents: Profile Data, Temperature=21 [C]
outlet
vent2
vent1
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-14
April 28, 2009
Inventory #002599

15. Starting Room Simulation in Workbench

WS3: Room Temperature Study
Starting Room Simulation in Workbench
Workshop Supplement
1. Drag CFX into the Project Schematic from the Component Systems
toolbox
2. Change the name of the system to room
3. Double-click Setup in the room system
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-15
April 28, 2009
Inventory #002599

16. Import Mesh

WS3: Room Temperature Study
Import Mesh
Workshop Supplement
The first step is to import the mesh that has already been created:
1. Right-click on Mesh in the Outline tree and select Import Mesh > ICEM
CFD
2. Select the file room.cfx5
3. Make sure the Mesh Units are in m and click Open to import the mesh
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-16
April 28, 2009
Inventory #002599

17. Create Domain

WS3: Room Temperature Study
Create Domain
Workshop Supplement
You can now create the computational domain:
1. Edit Default Domain from the Outline tree
2. On the Basic Settings tab, set the Fluid 1 Material setting to Air Ideal
Gas
3. Set the Buoyancy Option to Buoyant. Set the Buoyancy settings as
shown:
• Gravity X Dirn. = 0 [ m s^-2 ]
• Gravity Y Dirn. = 0 [ m s^-2 ]
• Gravity Z Dirn. = -g (first, click the Enter Expression icon )
• Buoy. Ref. Density = 1.185 [ kg m^-3 ]
Enabling Buoyancy allows for natural convection due to density
variations. The buoyancy force is a function of density variations
relative to the buoyancy reference density. Since density
variations can be very small, using a reference density help avoid
round-off errors. The reference density should be a typical fluid
density in the domain.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-17
April 28, 2009
Inventory #002599

18. Create Domain

WS3: Room Temperature Study
Create Domain
4.
5.
6.
7.
8.
9.
Workshop Supplement
Switch to the Fluid Models tab
Change the Heat Transfer Option to Thermal Energy
Change the Turbulence Model Option to Shear Stress Transport
Switch to the Initialisation tab
Check the Domain Initialisation box
Set the Temperature Option to Automatic with Value. Set the
Temperature to 21 [C]
For most cases, setting an initial condition for domain
temperature is not necessary since the solver can
automatically calculate initial conditions. However, if you input
a value that is closer to the final solution than what the solver
would automatically calculate, you will reach a converged
solution faster.
10. Click OK to commit the changes to the domain
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-18
April 28, 2009
Inventory #002599

19. Profile data initialization

WS3: Room Temperature Study
Profile data initialization
Workshop Supplement
1. Select Tools >Initialise Profile Data
and choose the Data File as
vent1.csv. Click OK
–
CFX-Pre reads the file and creates
functions that point to the variables
available in the file (see the User
Functions section in the Outline tree).
Boundary conditions can be set by
referencing these functions. E.g.
VENT1.Velocity u(x,y,z) refers to
the Velocity u value in the VENT1 function
with the local coordinate values x, y and z
passed in as the arguments. Any value
with the correct dimensions can be
passed in as an argument, but usually the
local coordinates are used.
2. Similarly initialise profile data for vent
2 by choosing vent2.csv
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-19
April 28, 2009
Inventory #002599

20. Create Boundary Conditions

WS3: Room Temperature Study
Create Boundary Conditions
Workshop Supplement
Now create the following boundary conditions:
1. vent1 Boundary Condition
–
–
–
–
Name: vent1
Boundary Type: Inlet
Location: VENT1
Select Use Profile Data and choose
VENT1 as the Profile Name
– Click Generate Values
– This will create expressions for the
Mass and Momentum option on the
Boundary Details tab that reference the
profile functions
– On the Boundary Details tab check that
the expressions make sense
– Heat Transfer Option: Static
Temperature
– Static Temperature: 21 [C]
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-20
April 28, 2009
Inventory #002599

21. Create Boundary Conditions

WS3: Room Temperature Study
Create Boundary Conditions
Workshop Supplement
2. vent2 Boundary Condition
–
–
–
–
–
Name: vent2
Boundary Type: Inlet
Location: VENT2
Select Use Profile Data and choose VENT2 as the Profile Name
Click Generate Values
• The Mass and Momentum Option will be automatically updated
– Heat Transfer Option: Static Temperature
– Static Temperature: 21 [C]
3. workers Boundary Condition
–
–
–
–
–
Name: workers
Boundary Type: Wall
Location: WORKERS
Heat Transfer Option: Temperature
Fixed Temperature: 37 [C]
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-21
April 28, 2009
Inventory #002599

22. Create Boundary Conditions

WS3: Room Temperature Study
Create Boundary Conditions
Workshop Supplement
4. outlet Boundary Condition
–
–
–
–
–
–
–
Name: outlet
Boundary Type: Opening
Location: OUTLET
Mass and Momentum Option: Opening Pres. and Dirn
Relative Pressure: 0 [Pa]
Heat Transfer Option: Opening Temperature
Opening Temperature: 21 [C]
5. monitors Boundary Condition
–
–
–
–
–
Name: monitors
Boundary Type: Wall
Location: monitors
Heat Transfer Option: Temperature
Fixed Temperature: 30 [C]
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-22
April 28, 2009
Inventory #002599

23. Create Boundary Conditions

WS3: Room Temperature Study
Create Boundary Conditions
Workshop Supplement
6. computerVent Boundary Condition
– Name: computerVent
– Boundary Type: Inlet
– Location: COMPUTER1VENT, COMPUTER2VENT, COMPUTER3VENT,
COMPUTER4VENT
– Mass and Momentum Option: Mass Flow Rate
– Mass Flow Rate: 0.132 [kg/s]
– Heat Transfer Option: Static Temperature
– Static Temperature: 40 [C]
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-23
April 28, 2009
Inventory #002599

24. Create Boundary Conditions

WS3: Room Temperature Study
Create Boundary Conditions
Workshop Supplement
7. computerIntake Boundary Condition
– Name: computerIntake
– Boundary Type: Outlet
– Location: COMPUTER1INTAKE, COMPUTER2INTAKE,
COMPUTER3INTAKE, COMPUTER4INTAKE
– Mass and Momentum Option: Mass Flow Rate
– Mass Flow Rate: 0.132 [kg/s]
– Mass Flow Update Option: Constant Flux
• This enforces a uniform mass flow across the entire boundary region, rather
than letting a natural velocity profile develop. It is used here to make sure the
flow rate through each intake is the same.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-24
April 28, 2009
Inventory #002599

25. Solver Control

WS3: Room Temperature Study
Solver Control
Workshop Supplement
1. Edit Solver Control from the Outline tree
– Due to nature of this flow it will take a long time for a steady-state condition
to be reached
2. Increase the Max. Iterations to 750
3. Change the Timescale Control to Physical Timescale
4. Set a Physical Timescale of 2 [s]
5. Enable the Conservation Target toggle
6. Click OK to commit the settings
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-25
April 28, 2009
Inventory #002599

26. Monitor Point

WS3: Room Temperature Study
Monitor Point
Workshop Supplement
Monitor points are used to monitor quantities of interest during the
solution. They should be used to help judge convergence. In this case
you will monitor the temperature of the air that exits through the outlet.
One measure of a converged solution is when this air has reached a
steady-state temperature.
1.
2.
3.
4.
5.
Edit Output Control from the Outline tree
Switch to the Monitor tab and enable the Monitor Options toggle
Under Monitor Points and Expressions, click the New icon
Enter the Name as temp
Set the Option to Expression
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-26
April 28, 2009
Inventory #002599

27. Monitor Point

WS3: Room Temperature Study
Monitor Point
Workshop Supplement
6. In the Expression Value field, type in:
massFlowAve(Temperature)@outlet
7. Click OK to create the Monitor Point
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-27
April 28, 2009
Inventory #002599

28. Write Solver File

WS3: Room Temperature Study
Write Solver File
Workshop Supplement
You can now save the project and proceed to write a definition file for
the Solver:
1. Close CFX-Pre to return to the Project window and save the project
The solution will take several hours to solve on one processor. To save
time, a results file is provided with this workshop. The Project
Schematic shows that the room Solution has not been completed, so
you cannot view the results in CFD-Post yet. To view the results for the
file provided you’ll need to add the results to the project.
2.
3.
4.
5.
Select File > Import from the main menu in Workbench
Set the file filter to CFX-Solver Results File
Select the results file provided with this workshop, room_001.res
Change the name of the system to room results …
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-28
April 28, 2009
Inventory #002599

29. Project Schematic

WS3: Room Temperature Study
Project Schematic
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
Workshop Supplement
WS3-29
April 28, 2009
Inventory #002599

30. CFX Solver Manager

WS3: Room Temperature Study
CFX Solver Manager
Workshop Supplement
Now you can view the solution for the previously solved case.
1. Right-click on Solution in the room results system and select Display
Monitors
2. Examine the residual plots for Momentum and Mass, Heat Transfer
and Turbulence
• The Residual Target of 1e-4 was met at about 270 iterations, but the solver
did not stop because the Conservation Target had not been met
3. Examine the User Points plot
• Air temperature leaving through the outlet did not start to reach a steady
temperature until >650 iterations. Using residuals as the only convergence
criteria is not always sufficient.
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-30
April 28, 2009
Inventory #002599

31. Residual and Monitor plot

WS3: Room Temperature Study
Residual and Monitor plot
Workshop Supplement
Residual plot
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
Monitor points
WS3-31
April 28, 2009
Inventory #002599

32. CFX Solver Manager

WS3: Room Temperature Study
CFX Solver Manager
Workshop Supplement
6. Check the Domain Imbalances at the end of the .out file for each
equation
• You can right click in the text monitor, select Find… and search for
“Domain Imbalance” to find the appropriate section
• An imbalance is given for the U-Mom, V-Mom, W-Mom, P-Mass and HEnergy equations
• It took 653 iterations to satisfy the Conservation Target of 1% for the HEnergy equation – see the Plot Monitor 1 tab
7. Close the Solver Manager
8. View the results in CFD-Post by double-clicking Results in the
Project Schematic from the room system
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-32
April 28, 2009
Inventory #002599

33. CFD-Post

WS3: Room Temperature Study
CFD-Post
Workshop Supplement
Start by creating a ZX Plane at Y = 1.2 [m]
1. Select Location > Plane from the toolbar
2. In the Details windows on the Geometry tab, set the Definition Method
to ZX Plane
3. Set Y to 1.2 [m]
4. On the Colour tab set Mode to Variable
5. Set Variable to Temperature
6. Set Range to Local and click Apply
• Observe the temperature distribution (for example, how the warm air collects
under the table)
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-33
April 28, 2009
Inventory #002599

34. CFD-Post

WS3: Room Temperature Study
CFD-Post
Workshop Supplement
Using the same procedure, create several other planes displaying the
temperature profile:
1. ZX Plane at Y = 2 [m]
2. ZX Plane at Y = 5.1 [m]
3. XY Plane at Z = 0.25 [m]
4. When finished observing the temperature distribution, uncheck the
visibility boxes of the planes that you created
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-34
April 28, 2009
Inventory #002599

35. CFD-Post

WS3: Room Temperature Study
CFD-Post
Workshop Supplement
Plot vector plots on the planes that you created:
1. Click Insert > Vector from the main menu
2. In the Details windows on the Geometry tab, set Location to Plane 2
and Symbols Size to 3.0 in Symbol tab
3. Click Apply
4. After observing the flow behavior on Plane 2, switch the Location to
Plane 4
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-35
April 28, 2009
Inventory #002599

36. Further Steps (Optional)

WS3: Room Temperature Study
Further Steps (Optional)
Workshop Supplement
Time permitting, you may want to try the following:
1. Observe the density variation at various planes
2. Create a streamline from each of the vents
• You may want to adjust the values on the Limits tab (Max. Segments)
3. Animate the streamlines
• Right-click on the Streamlines in the 3D viewer and select Animate
4. Create an isosurface based on different temperatures (e.g., 22 [C],
24 [C], etc.)
5. Calculate the areaAve of Wall Heat Flux on the workers
• Click Tools > Function Calculator
ANSYS, Inc. Proprietary
© 2009 ANSYS, Inc. All rights reserved.
WS3-36
April 28, 2009
Inventory #002599