You are viewing the documentation for an older COMSOL version. The latest version is available here.
PDF
Electronic Chip Cooling
Introduction
This model is an introduction to simulations of device cooling. A device (here a chip associated to a heat sink) is cooled by a surrounding fluid, air in this case. This tutorial demonstrates the following important steps:
•
Defining a heat rate on a domain using automatic volume computation.
•
Modeling the temperature difference between two surfaces when a thermally thick layer is present.
•
Including the radiative heat transfer between surfaces in a model.
In addition, this tutorial compares two approaches for modeling the air cooling. First, only the solid is represented and a convective cooling heat flux boundary condition is used to account for the heat transfer between the solid and the fluid. In a second step, the air domain is included in the model and a non-isothermal flow model is defined.
Model Definition
The modeled system describes an aluminum heat sink used for the cooling of an electronic chip, as shown in Figure 1.
Figure 1: Geometry of the heat sink and the electronic chip.
The heat sink represented in gray in Figure 1 is mounted inside a channel with a rectangular cross section. Such a setup is used to measure the cooling capacity of heat sinks. Air enters the channel at the inlet and exits the channel at the outlet. Thermal grease is used to improve the thermal contact between the base of the heat sink and the top surface of the electronic component. All other external faces are thermally insulated. The heat dissipated by the electronic component is equal to 5 W and is distributed through the chip volume.
The cooling capacity of the heat sink can be determined by monitoring the temperature in the electronic component.
The model solves a thermal balance for the electronic component, heat sink, and air flowing in the rectangular channel. Thermal energy is transferred by conduction in the electronic component and the aluminum heat sink. Thermal energy is transported by conduction and advection in the cooling air. Unless an efficient thermal grease is used to improve the thermal contact between the electronic component and the heat sink, the temperature field varies sharply there. The temperature is set at the inlet of the channel. The transport of thermal energy at the outlet is dominated by convection.
Initially, heat transfer by radiation between surfaces is neglected. This assumption is valid as the surfaces have low emissivity (close to 0), which is usually the case for polished metals. In a case where the surface emissivity is large (close to 1), the surface-to-surface radiation should be considered. This is done later in this tutorial, where the model is modified to account for surface-to-surface radiation at the channel walls and heat sink boundaries. Assuming that the surfaces have been treated with black paint, the surface emissivity is close to 1 in this second case.
The flow field is obtained by solving one momentum balance relation for each space coordinate (x, y, and z) and a mass balance equation. The inlet velocity is defined by a parabolic velocity profile for fully developed laminar flow. At the outlet, the normal stress is equal to the outlet pressure and the tangential stress is canceled. At all solid surfaces, the velocity is set to zero in all three spatial directions.
The thermal conductivity of air, heat capacity of air, and air density are all temperature-dependent material properties. You can find all of the settings in the physics interface for Conjugate Heat Transfer in COMSOL Multiphysics. The material properties, including their temperature dependence, are available in the Material Browser.
Results and Discussion
Modeling Using Convective Cooling Boundary Condition
In this part of the model, only the solid domains are represented. Instead of computing the flow velocity, pressure, and temperature in the air channel, a convective cooling boundary condition is used at the heat sink boundaries. The approach enables very quick computations, but its accuracy relies on the heat transfer coefficient that is used to define the convective cooling condition. In this configuration, an empirical value, 10 W/(m2·K), is used.
Next, to model the thermal contact between the heat sink and the chip three hypotheses are considered. In a first simulation an ideal contact is assumed.
Figure 2: Temperature plot of the heat sink for the first configuration.
Under ideal conditions, the maximum temperature in the chip is about 84 °C.
In the second simulation, a 50-µm-thick layer of air between the heat sink and the chip is assumed to create a thermal resistance.
Figure 3: Temperature plot of the heat sink for the second configuration.
The thermal resistance decreases the performance of the heat sink and the maximum temperature is close to 95 °C.
Finally, a third configuration is tested where the thin layer contains thermal grease instead of air.
Figure 4: Temperature plot.
The maximum temperature is close to the one observed in the first configuration with an ideal thermal contact. This means that the effect of the thermal resistance is greatly reduced by the thermal grease, which has a higher thermal conductivity than air.
Modeling Using Nonisothermal Flow in the Channel
Since the heat transfer coefficient is in general unknown, an alternative approach is suitable. In this part, a domain corresponding to the air channel is added to the geometry in order to compute the flow and the temperature field in the air. This leads to more computationally expensive simulations, but the approach is more general.
In Figure 5, the hot wake behind the heat sink is a sign of the convective cooling effects. The maximum temperature, reached in the electronic component, is about 96 °C.
Figure 5: The surface plot shows the temperature field on the channel walls and the heat sink surface.
Compared with the first approach (without the air domain), the results are different. This shows that using a heat transfer coefficient that is not well known, as in the first approach, leads to inaccurate results.
In the second step, the temperature and velocity fields are obtained when surface-to-surface radiation is included and the surface emissivities are large. Figure 6 shows that the maximum temperature, about 82 °C, is decreased by about 14 °C when compared to the first case in Figure 5. This confirms that radiative heat transfer is not negligible when the surface emissivity is close to 1.
Figure 6: The effects of surface-to-surface radiation on temperature. The surface plot shows the temperature field on the channel walls and the heat sink surface.
Application Library path: Heat_Transfer_Module/Tutorials,_Forced_and_Natural_Convection/chip_cooling
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>Heat Transfer in Solids and Fluids (ht).
3
Click Add.
4
Click Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click Done.
Global Definitions
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file chip_cooling.txt.
Geometry 1
Block 1 (blk1)
1
In 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 L_chip.
4
In the Depth text field, type L_chip.
5
In the Height text field, type H_chip.
6
Locate the Position section. In the z text field, type -H_chip.
7
Click Build Selected.
Part Libraries
1
In the Geometry toolbar, click Parts and choose Part Libraries.
2
In the Model Builder window, click Geometry 1.
3
In the Part Libraries window, select Heat Transfer Module>Heat Sinks>heat_sink_straight_fins in the tree.
4
Click Add to Geometry.
Geometry 1
Heat Sink - Straight Fins 1 (pi1)
1
In the Model Builder window, under Component 1 (comp1)>Geometry 1 click Heat Sink - Straight Fins 1 (pi1).
2
In the Settings window for Part Instance, locate the Input Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
n_fins_x
n_fins
4
Amount of fins in x-direction
X_fins_bottom
3[mm]
0.003 m
Fin dimension in x-direction, bottom
X_fins_top
2[mm]
0.002 m
Fin dimension in x-direction, top
4
Locate the Position and Orientation of Output section. Find the Coordinate system in part subsection. From the Work plane in part list, choose Work plane for heat sink base (wp11).
5
Find the Displacement subsection. In the xw text field, type -5[mm].
6
In the yw text field, type -5[mm].
7
Click to expand the Domain Selections section. In the table, enter the following settings:
Name
Keep
Physics
Contribute to
Heat sink base
 
√
None
Step domain
 
√
None
Array of fins
 
√
None
All
√
√
None
8
Click to collapse the Domain Selections section. Click to expand the Boundary Selections section. In the table, enter the following settings:
Name
Keep
Physics
Contribute to
Bottom boundary
 
√
None
Exterior
 
√
None
Exterior boundaries without heat sink base
√
√
None
All
 
√
None
9
Click to collapse the Boundary Selections section. In the Geometry toolbar, click Build All.
10
Click the Zoom Extents button in the Graphics toolbar.
11
In the Home toolbar, click Windows and choose Add Material from Library.
Add Material
1
Go to the Add Material window.
2
In the tree, select Built-In>Aluminum.
3
Click Add to Component 1.
4
In the tree, select Built-In>Silica glass.
5
Click Add to Component 1.
6
In the Home toolbar, click Add Material to close the Add Material window.
Materials
Silica glass (mat2)
1
Click the Zoom Extents button in the Graphics toolbar.
2
Click the Wireframe Rendering button in the Graphics toolbar.
3
Select Domain 3 only.
In order to easily reuse the selection of the domain corresponding to the chip, create a dedicated selection for it.
4
In the Settings window for Material, locate the Geometric Entity Selection section.
5
Click Create Selection.
6
In the Create Selection dialog box, type Chip in the Selection name text field.
7
Click OK.
8
In the Physics toolbar, click Ambient Thermal Properties.
Heat Transfer in Solids and Fluids (ht)
Heat Source 1
1
In the Physics toolbar, click Domains and choose Heat Source.
2
In the Settings window for Heat Source, locate the Domain Selection section.
3
From the Selection list, choose Chip.
4
Locate the Heat Source section. Click the Heat rate button.
5
In the P0 text field, type P0.
Heat Flux 1
1
In the Physics toolbar, click Boundaries and choose Heat Flux.
2
In the Settings window for Heat Flux, locate the Boundary Selection section.
3
From the Selection list, choose Exterior boundaries without heat sink base (Heat Sink - Straight Fins 1).
4
Locate the Heat Flux section. Click the Convective heat flux button.
First enter the heat transfer coefficient defined from a parameter.
5
In the h text field, type h0.
Then the external temperature is set to the ambient temperature defined in the ambient thermal properties node (default value is 293.15 K).
6
From the Text list, choose Ambient temperature (amth1).
7
In the Home toolbar, click Compute.
The computation takes a few seconds and about 1 GB of memory.
Results
Temperature (ht)
Two default plots are generated automatically. The first one shows the temperature profile on the boundaries, and the second one shows the isothermal surfaces.
Surface 1
1
In the Model Builder window, expand the Temperature (ht) node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose degC.
4
In the Temperature (ht) toolbar, click Plot.
Geometry 1
1
Click the Go to Default View button in the Graphics toolbar.
2
Click the Zoom Extents button in the Graphics toolbar.
Now update the model to evaluate the effect of the thermal contact between the chip and the heat sink. First assume a poor thermal contact due to a thin film of air between the chip and the heat sink.
Heat Transfer in Solids and Fluids (ht)
Thermal Contact 1
1
In the Physics toolbar, click Boundaries and choose Thermal Contact.
2
Select Boundary 15 only.
To facilitate the selection of this boundary in the following steps, create a dedicated selection for it.
3
In the Settings window for Thermal Contact, locate the Boundary Selection section.
4
Click Create Selection.
5
In the Create Selection dialog box, type Chip/Heat Sink Interface in the Selection name text field.
6
Click OK.
7
In the Settings window for Thermal Contact, locate the Thermal Contact section.
8
From the Contact model list, choose Equivalent thin resistive layer.
9
From the Specify list, choose Layer thermal conductivity and thickness.
10
In the ds text field, type 50[um].
Materials
Define the material (air) present at the interface between the chip and the heat sink.
1
In the Home toolbar, click Windows and choose Add Material from Library.
Add Material
1
Go to the Add Material window.
2
In the tree, select Built-In>Air.
3
Click Add to Component 1.
4
In the Home toolbar, click Add Material to close the Add Material window.
Materials
Air (mat3)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Geometric entity level list, choose Boundary.
3
From the Selection list, choose Chip/Heat Sink Interface.
4
In the Home toolbar, click Compute.
Results
Temperature (ht)
1
Click Compute.
The temperature plot is updated after the computation. Note that the presence of the thin layer of air between the chip and the heat sink induced more than a 10°C increase of the maximum temperature.
Now assume that thermal grease is used to avoid an air layer at the interface between the chip and the heat sink. Update the model in order to check how the cooling is improved by this change.
2
Click Windows and choose Add Material from Library.
Add Material
1
Go to the Add Material window.
2
In the tree, select Built-In>Thermal grease.
3
Click Add to Component 1.
4
In the Home toolbar, click Add Material to close the Add Material window.
Materials
Thermal grease (mat4)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Geometric entity level list, choose Boundary.
3
From the Selection list, choose Chip/Heat Sink Interface.
The red triangle in the Air material icon indicates that it is overridden by the Thermal grease material.
4
In the Home toolbar, click Compute.
Results
Temperature (ht)
The temperature plot is updated and shows the temperature distribution when thermal grease is used.
At this point we can evaluate the effect of the quality of the thermal contact. In the first computation, the thermal contact was assumed to be ideal and the maximum temperure was around 84°C. When accounting for a 50-µm-wide air layer the maximum temperature was close to 95°C. Using thermal grease to enhance the thermal contact seems efficient here as the maximum temperature is only slightly higher than the initial case of ideal thermal contact.
In the first part, we have been using a convective cooling boundary condition to account for the air flow cooling. While there are a number of geometrical configurations for which the heat transfer coefficient is known with very good accuracy, that is not the case for this particular heat sink geometry.
Modify the model to include the air channel in the geometry and to compute the air velocity. Then, you can accurately model the flow cooling without relying on any approximation of the heat transfer coefficient.
Geometry 1
Block 2 (blk2)
1
In 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 W_channel.
4
In the Depth text field, type D_channel.
5
In the Height text field, type H_channel.
6
Locate the Position section. In the x text field, type -(W_channel-40[mm])/2.
7
In the y text field, type -80[mm].
8
In the Geometry toolbar, click Build All.
9
Click the Zoom Extents button in the Graphics toolbar.
Define the material properties in the newly created channel domain.
Materials
Air (mat3)
1
In the Model Builder window, under Component 1 (comp1)>Materials right-click Air (mat3) and choose Duplicate.
This creates a new instance of the Air material that will be applied to the domain selection corresponding to the channel.
Air 1 (mat5)
1
In the Settings window for Material, locate the Geometric Entity Selection section.
2
From the Geometric entity level list, choose Domain.
3
Select Domain 1 only.
4
Click Create Selection.
5
In the Create Selection dialog box, type Air in the Selection name text field.
6
Click OK.
Component 1 (comp1)
In the Home toolbar, click Windows and choose Add Physics.
Add Physics
1
Go to the Add Physics window.
2
In the tree, select Fluid Flow>Single-Phase Flow>Laminar Flow (spf).
3
Click Add to Component in the window toolbar.
4
In the Home toolbar, click Add Physics to close the Add Physics window.
Laminar Flow (spf)
Specify that the flow interface is active only in the air channel.
1
In the Settings window for Laminar Flow, locate the Domain Selection section.
2
From the Selection list, choose Air.
Inlet 1
1
In the Physics toolbar, click Boundaries and choose Inlet.
2
Select Boundary 2 only.
3
In the Settings window for Inlet, locate the Boundary Selection section.
4
Click Create Selection.
5
In the Create Selection dialog box, type Inlet in the Selection name text field.
6
Click OK.
7
In the Settings window for Inlet, locate the Velocity section.
8
In the U0 text field, type U0.
Outlet 1
1
In the Physics toolbar, click Boundaries and choose Outlet.
2
Select Boundary 5 only.
3
In the Settings window for Outlet, locate the Boundary Selection section.
4
Click Create Selection.
5
In the Create Selection dialog box, type Outlet in the Selection name text field.
6
Click OK.
Heat Transfer in Solids and Fluids (ht)
Heat Flux 1
The boundaries where the heat flux condition was applied are no longer exterior boundaries, so the heat flux condition cannot be applied. Instead, a continuity condition is applied by default between the solid and the fluid domains.
Fluid 1
1
In the Model Builder window, under Component 1 (comp1)>Heat Transfer in Solids and Fluids (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 in Solids and Fluids (ht).
Inflow 1
1
In the Physics toolbar, click Boundaries and choose Inflow.
2
In the Settings window for Inflow, locate the Boundary Selection section.
3
From the Selection list, choose Inlet.
4
Locate the Upstream Properties section. From the Tustr list, choose Ambient temperature (amth1).
Outflow 1
1
In the Physics toolbar, click Boundaries and choose Outflow.
2
In the Settings window for Outflow, locate the Boundary Selection section.
3
From the Selection list, choose Outlet.
Component 1 (comp1)
Now add the Nonisothermal Flow multiphysics feature to couple the Heat Transfer in Solids and Laminar Flow interfaces. By doing this, you ensure in particular that the velocity field computed by the Laminar Flow interface is used by the Fluid 1 feature in the Heat Transfer interface. In addition, the temperature dependence of the material properties in the flow interface is then defined from the temperature field computed by the Heat Transfer interface.
1
In the Home toolbar, click Windows and choose Add Multiphysics.
Add Multiphysics
1
Go to the Add Multiphysics window.
2
In the tree, select Heat Transfer>Conjugate Heat Transfer>Laminar Flow.
3
Click Add to Component in the window toolbar.
4
In the Home toolbar, click Add Multiphysics.
Mesh 1
As this tutorial is intended to explore the heat transfer modeling capabilities, define a coarse mesh to speed up the computation. Note however that for accurate results, a finer mesh is needed.
1
In the Model Builder window, under Component 1 (comp1) click Mesh 1.
2
In the Settings window for Mesh, locate the Physics-Controlled Mesh section.
3
From the Element size list, choose Extremely coarse.
4
In the Home toolbar, click Compute.
The computation for this model takes a couple of minutes and about 2 GB of memory. The longer computational time is due to the extra degrees on freedom corresponding to the velocity, pressure, and temperature in the air domain.
The default temperature plot shows the temperature on all surfaces. In order to visualize the temperature on the heat sink boundary, hide some walls from the display.
Geometry 1
1
Click the Click and Hide button in the Graphics toolbar.
2
Click the Select Boundaries button in the Graphics toolbar.
3
In the Model Builder window, under Component 1 (comp1) click Geometry 1.
4
On the object fin, select Boundaries 1, 2, 4, and 5 only.
Results
Temperature (ht)
Now modify the model to include surface-to-surface radiation effects. First, add the Surface-to-Surface Radiation physics interface to the model. Then, study the effects of surface-to-surface radiation between the heat sink and the channel walls.
Add Physics
1
In the Home toolbar, click Add Physics to open the Add Physics window.
2
Go to the Add Physics window.
3
In the tree, select Heat Transfer>Radiation>Surface-to-Surface Radiation (rad).
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click Add Physics to close the Add Physics window.
Surface-to-Surface Radiation (rad)
1
Select Boundaries 1, 3, 4, 6, 7, 9, 11–16, 22, 24–29, 31–35, 37, and 39–44 only.
By default, the radiation direction is controlled by the opacity of the domains. The solid parts are defined as opaque while the fluid parts are transparent. You can change these settings by modifying or adding an Opaque subnode under the Solid and Fluid nodes.
When the Diffuse Surface boundary condition defines the radiation direction as opacity controlled (the default setting), the selected boundaries should be located between an opaque and a transparent domain. The exterior is defined as transparent by default. Change the default setting to make the exterior opaque and have the radiation direction automatically defined on the channel walls.
Opacity 1
1
In the Physics toolbar, click Domains and choose Opacity.
2
In the Settings window for Opacity, locate the Domain Selection section.
3
From the Selection list, choose All voids.
Diffuse Surface 1
1
Click the View All button in the Graphics toolbar.
2
In the Physics toolbar, click Add Multiphysics.
Add Multiphysics
1
Go to the Add Multiphysics window.
2
Find the Select the physics interfaces you want to couple subsection. In the table, enter the following settings:
Physics
Couple
Laminar Flow (spf)
 
3
In the tree, select Heat Transfer>Radiation>Heat Transfer with Surface-to-Surface Radiation.
4
Click Add to Component in the window toolbar.
5
In the Physics toolbar, click Add Multiphysics.
Multiphysics
Click the View Unhidden button in the Graphics toolbar.
Materials
Material 6 (mat6)
1
In the Materials toolbar, click Blank Material.
2
In the Settings window for Material, type Heat sink walls in the Label text field.
3
Locate the Geometric Entity Selection section. From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Exterior boundaries without heat sink base (Heat Sink - Straight Fins 1).
5
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Surface emissivity
epsilon_rad
0.9
1
Basic
Material 7 (mat7)
1
In the Materials toolbar, click Blank Material.
2
In the Settings window for Material, type Channel walls in the Label text field.
3
Locate the Geometric Entity Selection section. From the Geometric entity level list, choose Boundary.
4
Click the View All button in the Graphics toolbar.
5
Select Boundaries 1, 3, 4, and 44 only.
6
Click the View Unhidden button in the Graphics toolbar.
7
Locate the Material Contents section. In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Surface emissivity
epsilon_rad
0.85
1
Basic
In order to keep the previous solution and to be able to compare it with this version of the model, add a second stationary study.
8
In the Home toolbar, click Windows and choose Add Study.
Add Study
1
Go to the Add Study window.
2
Find the Studies subsection. In the Select Study tree, select General Studies>Stationary.
3
Click Add Study.
4
In the Home toolbar, click Add Study to close the Add Study window.
Study 2
Step 1: Stationary
1
In the Settings window for Stationary, click to expand the Values of Dependent Variables section.
2
Find the Initial values of variables solved for subsection. From the Settings list, choose User controlled.
3
From the Method list, choose Solution.
4
From the Study list, choose Study 1, Stationary.
5
In the Home toolbar, click Compute.
Results
Surface 1
1
In the Model Builder window, expand the Results>Temperature (ht) 1 node, then click Surface 1.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose degC.
Surface 2
1
In the Model Builder window, under Results>Temperature (ht) 1 click Surface 2.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose degC.
Surface 3
1
In the Model Builder window, under Results>Temperature (ht) 1 click Surface 3.
2
In the Settings window for Surface, locate the Expression section.
3
From the Unit list, choose degC.
4
In the Temperature (ht) 1 toolbar, click Plot.
By comparing this graph with the previous temperature graph we observe that the heat transfer by radiation induces a significant cooling and that the maximum temperature is about 10°C lower when thermal radiation is accounted for.