PDF
Microchannel Heat Sink
Introduction
This example models a microchannel heat sink mounted on an active electronic component. The model geometry is based on Pak et al.’s (Ref. 1) and Jang et al.’s papers (Ref. 2).
Thermal management has become a critical aspect of today’s electronic systems, which often include many high-performance circuits that dissipate large amounts of heat. Many of these components require efficient cooling to prevent overheating. Some of these components, such as processors, require a heat sink with cooling fins that are exposed to forced air from a fan. This discussion develops the model of an aluminum microchannel heat sink whose manifolds work as flow dividers to improve its cooling performance (see Figure 1).
This case examines the temperature field in the air, in the aluminum, and in the heat source. The air transports heat by convection and conduction. The aluminum heat sink transports thermal energy by pure conduction. The model accounts also for the thermal contact resistance between the heat sink and the electronic component.
Figure 1: Microchannel heat sink with manifolds.
Model Definition
The model geometry consists of three domains: the electronic component, the aluminum heat sink, and the cooling air. Due to symmetry considerations, it is sufficient to model only a small element of the entire geometry as shown in Figure 2. Symmetry boundary conditions would then complete the model definition. In particular, the surfaces labeled Inlet and Outlet represent one quarter of the actual inlet and outlet.
This simulation uses the Conjugate Heat Transfer interface to solve for the coupled flow field in the air domain and the temperature field in the entire geometry.
Figure 2: Model geometry with symmetries.
Boundary conditions
A laminar inflow profile with an average velocity of 0.85 m/s at the inlet is used together with a prescribed temperature of 22 °C. At the outlet the heat leaves through convection.
At the interface between the heat sink and electronic component, the Thermal Contact boundary condition is used. Thermal contact resistance is an important factor in the design of electronics cooling because it can significantly reduce a heat sink cooling performance. For more information about the thermal contact feature and its settings, read the theory section about the Thermal Contact feature in the Heat Transfer Module User’s Guide.
The surfaces of the heat sink and the ceramic heat source are not in perfect contact because of their roughness; air fills the gaps between the surfaces. Modeling the interface with the geometry of the rough surfaces would require a very dense mesh. An alternative, more practical, way of modeling the interface is to define a non-ideal thermal contact, that is representative for the interface. In this case, the joint conductivity is the sum of the gap conductance hg and the conductivity due to the contact surface properties hc. The latter depends on the contact pressure, surface roughness and microhardness and is described by the Cooper-Mikic-Yovanovich correlation (Ref. 3).
Results and Discussion
Figure 3 shows the velocity profile via magnitude field and arrow plot in the air domain.
Figure 3: Velocity profile in the air domain.
Figure 4 shows the resulting temperature field in the heat sink with velocity streamlines in the air domain.
Figure 4: Temperature field and velocity streamlines in the heat sink.
At the ceramic-aluminum imperfect contact region, a small temperature jump appears due to light contact pressure. The average jump evaluates to 0.7 K and the joint conductance of the interface is about 8900 W/(m2·K).
References
1. B.C. Pak, W.C. Chun, B.J. Baek and D. Copeland, “Forced Air Cooling by Using Manifold Microchannel Heat Sinks,” Advances in Electronic Packaging, ASME-EEP, vol. 19, no. 2, pp. 1837–1842, 1997.
2. S.P. Jang, S.J. Kim and K.W. Paik, “Experimental Investigation of Thermal Characteristics for a Microchannel Heat Sink Subject to an Impinging Jet, Using a Micro-Thermal Sensor Array,” Sensors and Actuators A: Physical, vol. 105, no. 2, pp. 211–224, 2003.
3. M.M. Yovanovich and E.E. Marotta, “Thermal Spreading and Contact Resistance,” Heat Transfer Handbook, A. Bejan and A.D. Kraus eds., John Wiley & Sons, 2003.
Application Library path: Heat_Transfer_Module/Power_Electronics_and_Electronic_Cooling/microchannel_heat_sink
Modeling Instructions
From the File menu, choose New.
New
In the New window, click Model Wizard.
Model Wizard
1
In the Model Wizard window, click 3D.
2
In the Select Physics tree, select Heat Transfer>Conjugate Heat Transfer>Laminar Flow.
3
Click Add.
4
Click Study.
5
In the Select Study tree, select Preset Studies for Selected Physics Interfaces>Stationary.
6
Click Done.
Geometry 1
1
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
2
In the Settings window for Geometry, locate the Units section.
3
From the Length unit list, choose mm.
Block 1 (blk1)
1
On the Geometry toolbar, click Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 0.2.
4
In the Height text field, type 2.85.
5
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
1.25
6
Click Build Selected.
Block 2 (blk2)
1
On the Geometry toolbar, click Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 0.1.
4
In the Height text field, type 1.4.
5
Locate the Position section. In the z text field, type 1.45.
6
Click Build Selected.
Difference 1 (dif1)
1
On the Geometry toolbar, click Booleans and Partitions and choose Difference.
2
Select the object blk1 only.
3
In the Settings window for Difference, locate the Difference section.
4
Find the Objects to subtract subsection. Select the Active toggle button.
5
Select the object blk2 only.
6
Click Build Selected.
Block 3 (blk3)
1
On the Geometry toolbar, click Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 0.2.
4
In the Height text field, type 1.85.
5
Locate the Position section. In the z text field, type 1.45.
6
Click Build Selected.
Difference 2 (dif2)
1
On the Geometry toolbar, click Booleans and Partitions and choose Difference.
2
Select the object blk3 only.
3
In the Settings window for Difference, locate the Difference section.
4
Find the Objects to subtract subsection. Select the Active toggle button.
5
Select the object dif1 only.
6
Select the Keep input objects check box.
7
Click Build Selected.
Delete Entities 1 (del1)
1
In the Model Builder window, right-click Geometry 1 and choose Delete Entities.
2
In the Settings window for Delete Entities, locate the Entities or Objects to Delete section.
3
From the Geometric entity level list, choose Object.
4
Select the object blk3 only.
5
Click Build Selected.
Block 4 (blk4)
1
On the Geometry toolbar, click Block.
2
In the Settings window for Block, locate the Size and Shape section.
3
In the Width text field, type 0.2.
4
In the Depth text field, type 0.5.
5
In the Height text field, type 0.45.
6
Locate the Position section. In the y text field, type 0.25.
7
In the z text field, type 2.85.
8
Click Build Selected.
Difference 3 (dif3)
1
On the Geometry toolbar, click Booleans and Partitions and choose Difference.
2
Select the object dif2 only.
3
In the Settings window for Difference, locate the Difference section.
4
Find the Objects to subtract subsection. Select the Active toggle button.
5
Select the object blk4 only.
6
On the Geometry toolbar, click Build All.
7
Click the Zoom Extents button on the Graphics toolbar.
Global Definitions
Define the parameters for the heat production and the contact pressure between the aluminum heat sink and the ceramic domain.
Parameters
1
On the Home toolbar, click Parameters.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
Q_in
5[W/cm^3]
5E6 W/m³
Heat production in ceramic
P_c
0.35[MPa]
3.5E5 Pa
Contact pressure
Select the materials from the built-in material library.
Add Material
1
On the Home toolbar, click Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Built-In>Air.
4
Click Add to Component in the window toolbar.
Add Material
1
Go to the Add Material window.
2
In the tree, select Built-In>Alumina.
3
Click Add to Component in the window toolbar.
Materials
Alumina (mat2)
1
In the Model Builder window, under Component 1 (comp1)>Materials click Alumina (mat2).
2
Select Domain 1 only.
Add Material
1
Go to the Add Material window.
2
In the tree, select Built-In>Aluminum 6063-T83.
3
Click Add to Component in the window toolbar.
Materials
Aluminum 6063-T83 (mat3)
1
On the Home toolbar, click Add Material to close the Add Material window.
2
In the Model Builder window, under Component 1 (comp1)>Materials click Aluminum 6063-T83 (mat3).
3
Select Domain 2 only.
Laminar Flow (spf)
1
In the Model Builder window, under Component 1 (comp1) click Laminar Flow (spf).
2
Select Domain 3 only.
3
In the Settings window for Laminar Flow, locate the Domain Selection section.
4
Click Create Selection.
5
In the Create Selection dialog box, type Air in the Selection name text field.
6
Click OK.
Inlet 1
1
On the Physics toolbar, click Boundaries and choose Inlet.
2
Select Boundary 14 only.
3
In the Settings window for Inlet, locate the Boundary Condition section.
4
From the list, choose Laminar inflow.
5
Locate the Laminar Inflow section. In the Uav text field, type 0.85.
The Entrance length value must be large enough so that the flow can reach a laminar profile. For a laminar flow, Lentr should be significantly greater than 0.06ReD, where Re is the Reynolds number and D is the inlet length scale. In this case, 1 mm is an appropriate value.
6
In the Lentr text field, type 1[mm].
Outlet 1
1
On the Physics toolbar, click Boundaries and choose Outlet.
2
Select Boundary 10 only.
Symmetry 1
1
On the Physics toolbar, click Boundaries and choose Symmetry.
2
Select Boundaries 7, 8, 17, 24, and 25 only.
Heat Transfer (ht)
Fluid 1
1
In the Model Builder window, under Component 1 (comp1)>Heat Transfer (ht) click Fluid 1.
2
In the Settings window for Fluid, locate the Domain Selection section.
3
From the Selection list, choose Air.
4
In the Model Builder window, click Heat Transfer (ht).
Heat Source 1
1
On the Physics toolbar, click Domains and choose Heat Source.
2
Select Domain 1 only.
3
In the Settings window for Heat Source, locate the Heat Source section.
4
In the Q0 text field, type Q_in.
Temperature 1
1
On the Physics toolbar, click Boundaries and choose Temperature.
2
Select Boundary 14 only.
3
In the Settings window for Temperature, locate the Temperature section.
4
In the T0 text field, type 22[degC].
Outflow 1
1
On the Physics toolbar, click Boundaries and choose Outflow.
2
Select Boundary 10 only.
Thermal Contact 1
1
On the Physics toolbar, click Boundaries and choose Thermal Contact.
2
Select Boundary 6 only.
3
In the Settings window for Thermal Contact, locate the Thermal Contact section.
4
From the hg list, choose Parallel-plate gap gas conductance.
5
Locate the Contact Surface Properties section. In the σasp text field, type 1.5[um].
6
In the masp text field, type 0.2.
7
In the p text field, type P_c.
8
In the Hc text field, type 1[GPa].
9
Click to expand the Gap properties section. Locate the Gap Properties section. From the kgap list, choose User defined.
Symmetry 1
1
On the Physics toolbar, click Boundaries and choose Symmetry.
2
Select Boundaries 1, 2, 4, 5, 7, 8, 15–17, and 22–25 only.
Mesh 1
The automatically generated mesh settings provide a good resolution for the fluid domains. In order to get a finer mesh in the solid domains, adjust the maximum element size for the solid domains.
1
In the Model Builder window, under Component 1 (comp1) right-click Mesh 1 and choose Edit Physics-Induced Sequence.
Size
1
In the Model Builder window, under Component 1 (comp1)>Mesh 1 click Size.
2
In the Settings window for Size, click to expand the Element size parameters section.
3
Locate the Element Size Parameters section. In the Maximum element size text field, type 0.09.
4
Click Build All.
5
On the Home toolbar, click Compute.
Results
Temperature (ht)
To reproduce the plot shown in Figure 4, follow the steps below.
Surface
1
In the Model Builder window, expand the Temperature (ht) node.
2
Right-click Surface and choose Delete. Click Yes to confirm.
Temperature (ht)
On the Temperature (ht) toolbar, click Slice.
Slice 1
1
In the Model Builder window, under Results>Temperature (ht) click Slice 1.
2
In the Settings window for Slice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Model>Component 1>Heat Transfer>Temperature>T - Temperature.
3
Locate the Coloring and Style section. From the Color table list, choose Thermal.
4
On the Temperature (ht) toolbar, click Plot.
Temperature (ht)
1
In the Model Builder window, under Results click Temperature (ht).
2
Click Streamline.
Streamline 1
1
In the Model Builder window, under Results>Temperature (ht) click Streamline 1.
2
In the Settings window for Streamline, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Model>Component 1>Laminar Flow>Velocity and pressure>u,v,w - Velocity field.
3
Locate the Selection section. Select the Active toggle button.
4
Select Boundary 14 only.
5
Locate the Streamline Positioning section. In the Number text field, type 25.
6
Locate the Coloring and Style section. From the Line type list, choose Tube.
7
In the Tube radius expression text field, type 0.005.
Color Expression 1
1
On the Temperature (ht) toolbar, click Color Expression.
2
In the Settings window for Color Expression, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Model>Component 1>Laminar Flow>Velocity and pressure>spf.U - Velocity magnitude.
3
On the Temperature (ht) toolbar, click Plot.
Velocity (spf)
The third default plot shows the velocity field in the air domain (see Figure 3).
Slice
1
In the Model Builder window, expand the Velocity (spf) node, then click Slice.
2
On the Velocity (spf) toolbar, click Plot.
Velocity (spf)
1
In the Model Builder window, under Results click Velocity (spf).
2
Click Arrow Volume.
Arrow Volume 1
1
In the Model Builder window, under Results>Velocity (spf) click Arrow Volume 1.
2
In the Settings window for Arrow Volume, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Model>Component 1>Laminar Flow>Velocity and pressure>u,v,w - Velocity field.
3
Locate the Arrow Positioning section. Find the X grid points subsection. In the Points text field, type 5.
4
Find the Z grid points subsection. In the Points text field, type 20.
5
Locate the Coloring and Style section. From the Color list, choose Black.
6
On the Velocity (spf) toolbar, click Plot.
Evaluate now the temperature jump and the joint conductance at the contact interface.
Surface Average 1
1
On the Results toolbar, click More Derived Values and choose Average>Surface Average.
2
In the Settings window for Surface Average, type Temperature Jump and Joint Conductance in the Label text field.
3
Select Boundary 6 only.
4
Locate the Expressions section. In the table, enter the following settings:
Expression
Unit
Description
up(T)-down(T)
K
Temperature jump
ht.tc1.hjoint
W/(m^2*K)
Joint conductance
The up and down operators return the temperature on each side of the contact boundary.
5
Click Evaluate.
The temperature jump at the interface is about 0.7 K, and the joint conductance is about 8900 W/(m²·K).