Electronics Cooling


1. Loading Geometry

Before we begin, download the following geometries Board, CPU and Pins

1. Click Load STL
2. Select all geometry files board.stl.gz cpu.stl.gz pins.stl.gz
3. Click Open

2. Geometry

After loading geometry, it will appear in the graphics window

1. Click Fit View button to zoom out the geometry

3. Fan geometry

Add fan geometry to the model. It will be placed above the CPU.

1. Click on the Box icon to add a new geometry
2. Double click on the new geometry and change its name to fan
3. Define box origin

Origin[m] 0.05 0.016 0.0115

4. Define box dimensions

Dimensions[m] 0.016 0.016 4e-03

4. Fan Inlet (I)

Now rotate the geometry of the model so that you can see the bottom side of the newly created fan. You will now select a face that will be subdivided from the fan as a separate boundary patch by the meshing tool.

1. Press Ctrl and select this bottom surface of the fan
2. Click on the Geometry Faces tab
3. Click on the Create New Face Group button
4. Select Create Group From 3D Selection from the list

5. Fan Inlet (II)

1. Double-click to rename newly created group to inlet

6. Outlet Tool

The last primitive geometry to create is a box that will be used as a tool to extract outlet patch from outer boundaries

1. Click on the Box button to add a new geometry
2. Double click on the new geometry and change its name to outlet_tool
3. Define box origin

Origin[m] 0.0845 0.0415 0

4. Define box dimensions

Dimensions[m] 6.5e-03 9e-03 8e-03

7. Enable Fan Meshing

Now set meshing parameters for the fan geometry

1. Go to Hex Meshing panel
2. Select fan geometry
3. Enable meshing on the fan geometry
4. Set mesh refinement on the geometry

Refinement Min 1 Max 3

8. Enable Board Geometry Meshing

Now set meshing parameters for rpi2 geometry

1. Select rpi2 geometry
2. Enable meshing on the rpi2 geometry
3. Set mesh refinement on the geometry

Refinement Min 2 Max 3

9. Enable CPU Geometry Meshing

You will now use similar meshing settings for the rpi2_cpu geometry

1. Select rpi2_cpu geometry
2. Enable meshing on rpi2_cpu geometry
3. Set mesh refinement on the geometry

Refinement Min 2 Max 4

10. Base Mesh Geometry

You will define outer boundaries of the computational domain now

1. Go to Base tab
2. Define the box size

Min[m] 0 0 0
Max[m] 0.085 0.056 0.0155

3. Define the number of axial divisions

Division 15 10 5

11. Base Mesh Boundaries

1. Click on the Patch button
2. Change boundary type to wall for all base mesh boundaries

12. Material Point in Solid

You need to tell the meshing algorithm where mesh for the solid region should be created

1. Go to Point tab
2. Specify location inside the CPU box

Material Point 0.055 0.02 5e-04

13. Meshing - Solid Region

Everything is set up now for the meshing of the solid region

1. Go to Mesh tab
2. Press Mesh button to start meshing process

14. Converting Solid to Sub-region

Before generating mesh for the fluid region, you must convert current mesh into sub-region. Otherwise, it would be overwritten by the new mesh

1. Go to MESH panel
2. Press Options button
3. Select Make sub-region option
4. Enter name solid for the sub-region
5. Click OK button

15. Solid Region Type

1. Expand region type options
2. Select Solid type for solid region

16. Material Point in Fluid

Once the solid region is created, you can move material point to anywhere inside the base mesh, but outside the solid region

1. Go to Hex Meshing panel
2. Go to Point tab
3. Specify location inside the fluid mesh

Material Point 0.055 0.02 5e-03

17. Meshing - Fluid Region

Everything is set up now for the meshing of the fluid region

1. Go to Mesh tab
2. Press Mesh button to start meshing process

18. Mesh

The mesh will be displayed in the graphics window

19. Extract outlet patch (I)

In the geometry setup, you created outlet_tool. You will now use this box to extract patch from boundary patch

1. Go to MESH panel
2. Click Options button next to boundaries patch
3. Select Extract From option

20. Extract outlet patch (II)

1. Pick outlet_tool from the list
2. Click Extract

New patch will appear on the list of boundaries

21. Extract outlet patch (III)

Now we have to rename newly created boundary

1. Double click on extracted_from_boundaries to rename it
2. Rename it to outlet

22. Converting Fluid to Sub-region

Now, after you used Extract tool on default mesh, you can convert it into sub-region. It’s important to note that extract operations are no longer available once the mesh is converted:

1. Press Options button for the default region
2. Click Make sub-region button
3. Enter name fluid for the sub-region
4. Click OK button

23. Create Region Interface

Two mesh regions are not coupled until you create a region interface. It will be further used to define which information is exchanged between regions:

1. Select rPi2_cpu in fluid
2. Ctrl + select rPi2_cpu in solid
3. Click Create Region Interface icon

24. Set Boundary Conditions

Set remaining boundary conditions

1. Select wall boundary type for boundaries and fan
2. Select patch boundary type for fan_inlet and outlet
3. Select wall boundary type for rPi2

25. Setup Solver

You will use chtMultiRegionSimpleFoam solver. This is a steady state solver that allows modeling of conjugate heat transfer and radiation.

1. Go to SETUP panel
2. Pick chtMultiRegionSimpleFoam from the list of available solvers
3. Select solver

26. Radiation Setup

We will first run a simulation without taking radiative heat transfer into account. However, it is important to set up all radiation model parameters now.
(these parameters cannot be changed later without resetting simulation)

1. Go to Radiation panel
2. Uncheck Enable Radiation
3. Pick Surface To Surface model from the drop-down list
4. Increase the Max rays number to 3000000

27. Thermophysical Properties of Solid

We will define now the thermodynamic properties of solid material

1. Go to Thermo panel
2. Select solid region
3. Click Material Database button
4. Select aluminium material
5. Click Apply

28. Thermophysical Properties of Fluid (I)

We will define now the thermodynamic properties of fluid material

1. Select fluid region
2. Click Material Database button
3. Select air material
4. Click Apply

29. Thermophysical Properties of Fluid (II)

1. Pick Incompressible Perfect Gas Equation of State

30. Turbulence

For turbulence modeling, we will use Realizable k-ε model

1. Go to Turbulence panel
2. Select RANS turbulence formulation
3. Select Realizable k-ε model

31. Solution - Solvers

We will now adjust solver tolerance threshold of the enthalpy equation in the solid region in order to achieve better convergence

1. Go to Solution panel
2. Select h (solid) tab
3. Expand solver options
4. Lower solver tolerance to 1e-08

32. Solution - SIMPLE

We will now adjust SIMPLE algorithm settings in order to achieve better convergence

1. Go to the SIMPLE tab
2. Increase number of Non-Orthogonal Correctors to 2

33. Solution - Relaxation

We will now adjust relaxation parameters in order to achieve better convergence

1. Go to Relaxation tab
2. Adjust relaxation coefficients

h(solid) 1
p-ρgh 0.3
U 0.4
h 1
ρ 0.8
k 0.8
ε 0.8

34. Solution - Limits

We will now adjust the limits of temperature fields in order to narrow the convergence space of the solution

1. Go to Limits tab
2. Enable Temperature Limits
3. Adjust minimum and maximum temperature to a reasonable range

T min 290
T max 600

35. Cell Zones

Now set heat source term in the CPU volume. In this tutorial, we assume that only the CPU produces the heat of power of 0.25 W and its volume is about 200 mm3:

1. Go to Cell Zones setup
2. Enable Source term for all cells in solid
3. Click Manage terms
4. Enable h equation source term
5. Set explicit source term to 1250000

36. Boundary Conditions - Inlet (Flow)

On the inlet, we will set constant air inflow

1. Go to Boundary Conditions panel
2. Change boundary condition for fan_inlet to Velocity Inlet
3. Set inlet velocity Reference Value[m/s] to 0.1

37. Boundary Conditions - Outlet (Turbulence)

We will now set boundary conditions on the outlet

1. Change boundary condition for outlet to Pressure Outlet
3. Switch to Turbulence tab
4. Pick Zero gradient type for k equation
5. Pick Zero gradient type for ε equation

38. Boundary Conditions - Solid Region (Thermal)

We will now enable radiation coupling on the solid side of the interface

1. Click on rPi2_cpu in solid
2. Select Coupled Temperature and Radiation type

39. Boundary Conditions - Fluid Region (Thermal)

Next, enable radiation coupling on the fluid side of the interface

1. Click on rPi2_cpu in fluid
2. Switch to Thermal tab
3. Select Coupled Temperature and Radiation type

40. Start Simulation

The case is set up. To run the simulation

1. Go to Run panel
2. Set Number of Iterations to 800
3. Run simulation

41. Start Postprocessing - ParaView

Start ParaView software to display results

1. Go to Postprocessing panel
2. Start ParaView

42. ParaView - Load Results

1. Click Last Frame to select the latest result set
2. Click Apply to load results

43. ParaView - Display Temperature Contour (I)

We will now plot temperature contour on the circuit board again. We will use the same scale, so the differences in results are more evident

1. Click on Mesh Regions in the Properties tab to select all regions
2. Uncheck fluid/boundaries
3. Uncheck fluid/internalMesh
4. Click Apply

44. ParaView - Display Temperature Contour (II)

1. Select contour coloring variable to T
2. Click Rescale to Data Range

45. ParaView - Display Temperature Contour (III)

Results are displayed in the graphics window. Note that the maximum temperature in the domain is 362 K.

46. Radiation Setup

We will now enable radiation equation in our simulation. To do this, close Paraview and go back to SimFlow

1. Go to Radiation panel
2. Select Enable Radiation Equations model

47. Start Simulation with Radiation

The case is set up. To run the simulation

1. Go to Run panel
2. Set Number of Iterations to 2000
3. Run simulation

48. ParaView - Start Postprocessing (with Radiation)

Start ParaView software to display results

1. Go to Postprocessing panel
2. Start ParaView

49. ParaView - Load Results (with Radiation)

1. Click Last Frame to select the latest result set
2. Click Apply to load results

50. ParaView - Display Temperature Contour (with Radiation) (I)

You will now plot temperature contour on the circuit board again. You will use the same scale, so the differences in results are more evident

1. Click on Mesh Regions in the Properties tab to select all regions
2. Uncheck fluid/boundaries
3. Uncheck fluid/internalMesh
4. Click Apply

51. ParaView - Display Temperature Contour (with Radiation) (II)

1. Select contour coloring variable to T
2. Click Rescale to Custom Data Range
3. Set minimum and maximum value

Min 300 Max 362

4. Click Rescale

52. ParaView - Display Temperature Contour (with Radiation) (III)

Results are displayed in the graphics window. Note that in this case, the maximum temperature in the domain is 344 K, which is 18 K lower than in the previous simulation.

53. ParaView - Radiative Heat Flux (I)

Radiation plays an important role in this scenario. Therefore, our last task will be to display radiative heat flux mapped on the Raspberry Pi 2 geometry

1. Set contour coloring variable to qr(partial)
2. Uncheck solid/rPi2_CPU and solid/internalMesh
4. Click Apply

54. ParaView - Radiative Heat Flux (II)

Results are displayed in the graphics window.

This concludes this tutorial.

Note that this tutorial is meant only to demonstrate capabilities of the software and not to solve the problem in the best possible way. Therefore, some assumptions are taken to keep case setup time and computational time low. In particular, to refine the model, one could in first place consider setting more suitable emissivity coefficients for materials used.

This website uses cookies to offer you the best experience online. By continuing to use our website, you agree to the use of cookies.