1. Workshop 6 Electronics Cooling with Natural Convection and Radiation
Introduction to CFX

2. Goals
This workshop models the heat dissipation from a hot electronics component fitted to a printed circuit board (PCB) via a finned heat sink. The PCB is fitted into a casing, which is open at the top and bottom.
Initially only the heat transfer via convection and conduction will be modelled. The effect of thermal radiation will then be included at a later stage.

3. Loading Mesh (Workbench)
Open a new Workbench project and save it as HeatSink.wbpj
Look in the Component Systems section of the toolbox and drag a CFX system onto the Project Schematic
Double-click Setup to start CFX-Pre
In CFX-Pre, right-click Mesh and select Import Mesh > ANSYS Meshing
Select HeatSink.cmdb and click Open

4. Options
In the tree expand Case Options, double-click General and ensure that Automatic Default Domains is switched on and Automatic Default Interfaces is active.
Set the Interface Method to One Per Domain Pair. Click OK.
Separate interfaces are required for each domain because when radiation is added, emissivity will be set differently at each domain interfaces

5. Create Fluid Domains
First add a domain for the fluid region. The effects of buoyancy must be included, as the flow is driven by natural convection. The buoyancy reference density represents the density at the ambient conditions.
Right-click on Flow Analysis 1 and insert a new domain named Fluid
Open the details for Fluid and set the Location to Fluid
Set the Material to Air Ideal Gas
Switch the Buoyancy option to Buoyant and set the directional components to (0, -g, 0)
Click on the expression button to enter –g
Set the Reference Density to [kg m^-3]
Click the Fluid Models tab
Set Heat Transfer to Thermal Energy and Turbulence to None (Laminar)
Click OK

6. Creating Materials
CFX contains a library of many materials, but for this case we will create user materials for the component and Printed Circuit Board (PCB).
In the tree right-click on Materials and select Insert > Material. Name it ComponentMat
Define the material as a Pure Substance in the CHT Solids Material Group
Enable Thermodynamic State and select Solid
This must be set to allow it to be used in a solid domain
Click the Material Properties tab and set Density to 1120 [kg m^-3]
Select Specific Heat Capacity and set it to 1400 [J kg^-1 K^-1]
Expand Transport Properties and set Thermal Conductivity to 10 [W m^-1 K^-1]
Select OK

7. Creating Materials Repeat steps 1-7 to create PCBMat using
Density = 1250 [kg m^-3]
Specific Heat Capacity = 1300 [J kg^-1 K^-1]
Thermal Conductivity = 0.35 [W m^-1 K^-1]

8. Create Solid Domains
This case contains three different solid parts that use different materials. Each part will be created as a different domain.
Insert a new domain called HeatSink
Set the Location to HeatSink
Set the Domain Type to Solid Domain with the Material set to Aluminium
Click OK to create the domain
Note that an interface between the two domains is automatically created
Repeat steps 1-4 to create a solid domain called Component located at IC using the Material ComponentMat, and a further solid domain called PCB located at PCB using PCBMat
When all 4 domains are created the Default Domain will automatically be removed from the tree. Separate interfaces between each domain will have been automatically created, rather than combined into a single interface.

9. Adding Energy Source
The component is generating 75 [W] of heat which must be added to the simulation. To add this energy source in CFX, a subdomain must be created.
In the tree right-click on the Component domain and select Insert > Subdomain, using the name Chip
Set the Location to IC so the subdomain occupies the whole of the Component domain
Switch to the Sources tab and check the Sources box and the Energy box
Set the Option to Total Source, enter 75 [kg m^2 s^-3] then click OK

10. Boundary Conditions
For this case all of the heat will be extracted by the air passing over the heat exchanger so all solid walls will be defined using adiabatic settings. Within the simulation heat can pass between all of the solid and fluid domains because interfaces have been automatically created.
To allow air to enter or leave the simulation domain, the top and bottom face of the fluid domain are defined as openings.
Right-click on the Fluid domain and insert a new boundary called Walls and set the Boundary Type to Wall
Set the Location to Wall
Switch to the Boundary Details tab and check that Heat Transfer is set to Adiabatic then click OK
In the PCB domain rename PCB Default to PCBwalls and check that Heat Transfer is set to Adiabatic

11. Boundary Conditions
In the Fluid domain rename Fluid Default to Openings and check that the Location is set to be the two ends of the fluid domain
In the Basic Settings tab change the Boundary Type to Opening
In the Boundary Details tab set the Mass and Momentum option to Opening Pres. and Dirn with a relative pressure of 0 [Pa]
Set Heat Transfer to Opening Temperature at 45 [C]
The Opening Pressure and Opening Temperature options set Total values when flow is entering the domain and Static values when flow is leaving.
This is appropriate when the flow outside the domain is accelerated from rest before entering the domain but will have a velocity when leaving.

12. Solver Control
From the tree right-click Solver Control and select Edit
Increase the Max. Iterations to 500
Leave the Fluid Timescale Control set to Auto Timescale
Leave Solid Timescale set to Auto Timescale
Note that solid regions will use a much larger timescale than fluid regions because only the energy equation is being calculated within the solid
Click OK

13. Radiation Setup
The next step is to redefine the model to include radiation effects. This will be set up as a second analysis that can be run after the convection only case using results from the initial simulation as starting conditions. This reduces the overall computational time, as the convection only case will be much closer to the end solution.
Most of the settings will be the same as the original analysis so the first step will be to make a duplicate analysis.
Right-click on Flow Analysis 1 and rename it to Convection
Right-click on Convection and select Duplicate
Rename Copy of Convection to Radiation
This will form the basis of the radiation case

14. Adding Radiation to the Air Domains
The effects of radiation need to be included in the new analysis. In this case, the surface-to-surface model will be used so radiation is only passed from wall to wall and the fluid does not participate in any way. This saves computational time and is appropriate since air will not absorb or emit significant thermal radiation on these length scales.
In the Radiation analysis, edit the Fluid domain
Switch to the Fluid Models tab
Under Thermal Radiation set the Option to Discrete Transfer
Set Transfer Mode to Surface to Surface
Click OK

15. Updating the Boundary Conditions.
Adding radiation will produce an error because additional information is now required at the Openings boundary.
Edit the boundary Openings. Make sure that it is the copy from the Radiation Flow Analysis that is being edited
Click the Boundary Details tab and see that Thermal Radiation has been added and is set to Local Temperature
Click OK to accept this addition to the boundary condition
As the default value was all that was required in this case an alternative method of correcting this error would have been to right-click on the error message and select Auto Fix Physics.

16. Radiation Emissivity
Different materials will have different radiation emissivity values. These can be set at each of the boundaries around the Fluid domain within the Radiation analysis. The emissivity of a surface is a function of the material, surface finish and any coatings that may have been applied as well as local temperature and the radiation wavelength.
In the Fluid domain find the interface boundary that connects the HeatSink to the fluid
Hint: boundaries are highlighted in the viewer when selected
Open up that boundary and in the Boundary Details tab change Emissivity to 0.3 then click OK

17. Radiation Emissivity
Note that each interface object is shown at the flow analysis level. There are two interface boundaries (at the domain level) associated with each interface object. Here we are editing the emissivity values for the interface boundaries in the fluid domain. The interface boundaries in the solid domains do not have an emissivity, because there is no radiation in the solid domain (they are opaque!).
Find the interface boundary in the Fluid domain connecting the Component and Fluid domains and set Emissivity to 0.9
Find the interface connecting the PCB to the Fluid domain and set Emissivity to 0.9
Open the boundary Walls and set Emissivity to 0.9

18. Defining Configurations
CFX-Pre now contains two separate setups for this project. It is necessary to indicate the order in which they run and how they are linked. This is achieved by setting up configurations. (Note that you could run each case separately, manually starting the radiation case from the convection solution.)
In the main tree expand Simulation Control then right-click on Configurations and select Insert > Configuration, accepting the default name
In the General Settings tab set the Flow Analysis to Convection and Activation Condition 1 to Start of Simulation
Click OK

19. Defining Configurations
Insert a second configuration and set the Flow Analysis to Radiation. Set the Activation Condition to End of Configuration, and set Configuration Names to Configuration 1
Switch to the Run Definition tab, select Configuration Execution Control then Initial Values Specification. Set the option to Configuration Results, using Configuration 1
Click OK
The convection case will run first, then when it finishes the .res file it created will be used to initialise the radiation simulation.

20. Running the Simulation
Select File > Quit to exit CFX-Pre
Save the Project
In the Project Schematic, right-click on Solution and select Update
While the solver is running right-click on Solution again and select Display Monitors to check on progress

21. Running the Simulation
This case uses a multi-configuration setup so the first screen will show the global progress by showing which configuration is being run.
Change the Workspace from the current run to Configuration1_001
The standard out file and residuals are displayed
This run will take a while to run so after a few iterations stop the run and the results provided will be used
Close the Solver Manager

22. Open CFD-Post
The results field in the existing CFX module is associated with the partially calculated results from your setup. To analyse the existing results you will add a new results field to the project.
From the Component Systems section of the Toolbox drag a Results system onto the Project Schematic
Right-click on the Results cell (B2) and select Edit
When CFD-Post opens, select File > Load Results and select HeatSink.mres. Use the option Load complete history as: Separate cases

23. Case Comparison
The case comparison tool allows two different setups to be shown side by side and any differences between the two cases identified.
In the tree edit Case Comparison
Enable the check-box Case Comparison Active and check that Case 1 is set to Configuration 1 and Case 2 is set to Configuration 2
In the viewer a new view is created to display the difference between the convection only case and the case including radiation
Click Apply to enter comparison mode

24. Temperature
Temperature will be a key variable for any electronics cooling application so it will be displayed in several locations, such as within the flow, on the surfaces of the solid region and by extracting the maximum temperature within the component. When these plots are created they appear in the User Locations and Plots section of the tree.
Create a YZ plane using Location > Plane. Name it Centre, set X to 0 [m] and colour using the variable Temperature.
Create a contour plot using Insert > Contour or by clicking on Use the fluid-solid interfaces as the location (use the ‘…’ icon and Ctrl key to select multiple locations from both configurations). Set the Variable to Temperature using the Global Range.

25. Temperature
Move to the function calculator using the icon on the toolbar. Set the options to: Function = maxVal Location = Component Case = All Cases Variable = Temperature
Click Calculate
Note that with radiation (Configuration 2) the temperature in the solid is significantly lower than when radiation was not included. The cooling of the component is mirrored with an increase in the temperature of the walls around the fluid zone. This can be seen if you plot the temperature on the walls or use the Function Calculator with the areaAve function.

26. Flow Displays
To show the flow patterns a range of methods can be used including streamlines, vector plots and isosurfaces.
Switch off the visibility of the existing plots
Insert an isosurface using Location > Isosurface and set the Variable to Velocity with a value of 0.5 [m s^-1]
Gradually reduce the isosurface value to 0.2 [m s^-1] and notice that for the radiation case higher speed flow can be observed close to the fluid walls as well as the PCB

27. Flow Displays
Insert a vector plot using Insert > Vector or click on
Set the location to Centre. Change the sampling to Equally Spaced with 1000 points
If you wish to see the pattern in the slow speed sections try going to the Symbol tab and select Normalize Symbols
Insert streamlines using Insert > Streamlines or by clicking on
Set Start From to Openings
Apply 100 equally spaced points and set the Direction to Forward and Backward