Created in COMSOL Multiphysics 6.

Electronic Chip Cooling

This model is licensed under the COMSOL Software License Agreement 6.3.
All trademarks are the property of their respective owners. See www.comsol.com/trademarks.
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 nonisothermal 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.

2 | ELECTRONIC CHIP COOLING

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.

3 | ELECTRONIC CHIP COOLING

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 85°C.

4 | ELECTRONIC CHIP COOLING

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.

5 | ELECTRONIC CHIP COOLING

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.

6 | ELECTRONIC CHIP COOLING

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 85°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 75°C, is decreased by about 10°C when compared to the

7 | ELECTRONIC CHIP COOLING

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.

8 | ELECTRONIC CHIP COOLING

5 In the Select Study tree, select General Studies > Stationary.
6 Click Done.

GLOBAL DEFINITIONS

Parameters 1
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 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.

9 | ELECTRONIC CHIP COOLING

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 xwi text field, type -5[mm].
6 In the ywi 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   None
base
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.

10 | ELECTRONIC CHIP COOLING

11 In the Model Builder window, click Geometry 1.

ADD MATERIAL
1 In 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 > Aluminum.
4 Right-click and choose Add to Component 1 (comp1).
5 In the tree, select Built-in > Silica glass.
6 Right-click and choose Add to Component 1 (comp1).
7 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.

11 | ELECTRONIC CHIP COOLING

4 In the Settings window for Material, locate the Geometric Entity Selection section.
5 Click Create Selection.
6 In the Create Selection dialog, type Chip in the Selection name text field.
7 Click OK.

DEFINITIONS

Ambient Properties 1 (ampr1)

In the Physics toolbar, click Shared Properties and choose Ambient 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. From the Heat source list, choose Heat rate.
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. From the Flux type list, choose Convective heat flux.
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
Properties 1 node (the default value is 293.15 K).
6 From the Text list, choose Ambient temperature (ampr1).
7 In the Home toolbar, click Compute.
The computation takes a few seconds and about 1 GB of memory.

RESULTS
Change the unit of the temperature results to degrees Celsius.

12 | ELECTRONIC CHIP COOLING

Preferred Units 1
1 In the Results toolbar, click Configurations and choose Preferred Units.
2 In the Settings window for Preferred Units, locate the Units section.
3 Click Add Physical Quantity.
4 In the Physical Quantity dialog, select General > Temperature (K) in the tree.
5 Click OK.
6 In the Settings window for Preferred Units, locate the Units section.
7 In the table, enter the following settings:

Quantity Unit Preferred unit

Temperature K °C

8 Click Apply.

Temperature (ht)
The automatically generated default plot shows the temperature in the domain. Modify
this plot to display the temperature at the interface between the chip and the heat sink by
applying the existing domain selections to the volume plot.

Selection 1
1 In the Model Builder window, expand the Temperature (ht) node.
2 Right-click Volume 1 and choose Selection.
3 In the Settings window for Selection, locate the Selection section.
4 From the Selection list, choose Chip.

Volume 2
Right-click Volume 1 and choose Duplicate.

Selection 1
1 In the Model Builder window, expand the Volume 2 node, then click Selection 1.
2 In the Settings window for Selection, locate the Selection section.
3 From the Selection list, choose All (Heat Sink - Straight Fins 1).

Volume 2
1 In the Model Builder window, click Volume 2.
2 In the Settings window for Volume, click to expand the Title section.
3 From the Title type list, choose None.
4 Click to expand the Inherit Style section. From the Plot list, choose Volume 1.

13 | ELECTRONIC CHIP COOLING

Filter 1
1 Right-click Volume 2 and choose Filter.
2 In the Settings window for Filter, locate the Element Selection section.
3 In the Logical expression for inclusion text field, type x>0.02.
4 In the Temperature (ht) toolbar, click Plot.

Compare with the temperature plot shown above.

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.

14 | ELECTRONIC CHIP COOLING

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, 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.

ADD MATERIAL
1 In the Materials 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 Right-click and choose Add to Component 1 (comp1).
5 In the Materials 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.

15 | ELECTRONIC CHIP COOLING

RESULTS

Temperature (ht)

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.

ADD MATERIAL
1 In 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 > Thermal grease.
4 Right-click and choose Add to Component 1 (comp1).
5 In the Home toolbar, click Add Material to close the Add Material window.

16 | ELECTRONIC CHIP COOLING

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 temperature
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

17 | ELECTRONIC CHIP COOLING

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 airflow 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 1 (mat5)
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.
2 In the Settings window for Material, locate the Geometric Entity Selection section.
3 From the Geometric entity level list, choose Domain.
4 Select Domain 1 only.
5 Click Create Selection.

18 | ELECTRONIC CHIP COOLING

6 In the Create Selection dialog, type Air in the Selection name text field.
7 Click OK.

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 Fluid Flow > Single-Phase Flow > Laminar Flow (spf).
4 Click the Add to Component 1 button in the window toolbar.
5 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, type Inlet in the Selection name text field.
6 Click OK.
7 In the Settings window for Inlet, locate the Boundary Condition section.
8 From the list, choose Fully developed flow.
9 Locate the Fully Developed Flow section. In the Uav 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, type Outlet in the Selection name text field.
6 Click OK.

19 | ELECTRONIC CHIP COOLING

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, click Fluid 1.
2 In the Settings window for Fluid, locate the Domain Selection section.
3 From the Selection list, choose Air.

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 (ampr1).

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.

ADD MULTIPHYSICS
1 In the Home toolbar, click Add Multiphysics to open the Add Multiphysics window.
2 Go to the Add Multiphysics window.
3 In the tree, select Heat Transfer > Conjugate Heat Transfer > Laminar Flow.
4 Click the Add to Component button in the window toolbar.
5 In the Home toolbar, click Add Multiphysics to close the Add Multiphysics window.

20 | ELECTRONIC CHIP COOLING

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 Settings window for Mesh, locate the Physics-Controlled Mesh section.
2 From the Element size list, choose Extremely coarse.
3 In the table, clear the Use checkbox for Geometric Analysis, Detail Size.
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.
Add a plot from the Result Templates showing temperature and velocity field and hide
some walls from the display to make visible the temperature on the heat sink and on the
channel walls and the flow structure.

RESULT TEMPLATES
1 In the Results toolbar, click Result Templates to open the Result Templates window.
2 Go to the Result Templates window.
3 In the tree, select Study 1/Solution 1 (sol1) > Nonisothermal Flow 1 >
Temperature and Fluid Flow (nitf1).
4 Click the Add Result Template button in the window toolbar.
5 In the Results toolbar, click Result Templates to close the Result Templates window.

GEOMETRY 1
1 Click the Click and Hide button in the Graphics toolbar.
2 On the object fin, select Boundaries 1, 2, 4, and 5 only.

RESULTS

Solid Temperature
In the Model Builder window, expand the Results > Temperature and Fluid Flow (nitf1) node.

Filter 1
1 In the Model Builder window, expand the Results > Temperature and Fluid Flow (nitf1) >
Fluid Flow node, then click Filter 1.
2 In the Settings window for Filter, locate the Element Selection section.

21 | ELECTRONIC CHIP COOLING

3 In the Logical expression for inclusion text field, type spf.U>1.2*nitf1.Uave.
4 In the Temperature and Fluid Flow (nitf1) toolbar, click Plot.
Duplicate this plot and keep only temperature subnodes to see better the temperature
distribution.

Temperature of the channel walls and heat sink

1 In the Model Builder window, right-click Temperature and Fluid Flow (nitf1) and choose
Duplicate.
2 In the Settings window for 3D Plot Group, type Temperature of the channel walls
and heat sink in the Label text field.

3 Locate the Color Legend section. Clear the Show units checkbox.

Fluid Flow
1 In the Model Builder window, expand the Temperature of the channel walls and heat sink
node.
2 Right-click Fluid Flow and choose Delete.

Temperature of the channel walls and heat sink

1 In the Model Builder window, under Results click
Temperature of the channel walls and heat sink.

22 | ELECTRONIC CHIP COOLING

2 In the Temperature of the channel walls and heat sink toolbar, click Plot.

Now modify the model to include surface-to-surface radiation effects. First, add the
Surface-to-Surface Radiation 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 the Add to Component 1 button in the window toolbar.
5 In the Home toolbar, click Add Physics to close the Add Physics window.

SURFACE-TO-SURFACE RADIATION (RAD)

1 In the Settings window for Surface-to-Surface Radiation, locate the Boundary Selection
section.
2 From the Selection list, choose Exterior boundaries without heat sink base (Heat Sink -
Straight Fins 1).

23 | ELECTRONIC CHIP COOLING

3 To add the channel walls, click the Paste Selection button and type 1 3 4 44 (note that
boundaries 1 and 4 have been hidden previously and are not visible in the graphics
window).
The interface selection now contains boundaries 1, 3, 4, 6, 7, 9, 11–16, 22, 24–29, 31–
35, 37, and 39–44.
By default the radiation direction is controlled by the opacity of the domains. The solid
parts are automatically defined as opaque while the fluid parts are transparent. You can
change this setting using the Opacity feature in the Surface-to-Surface Radiation interface.
When the Diffuse Surface boundary condition defines Emitted 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 In the Model Builder window, click Diffuse Surface 1.
2 In the Settings window for Diffuse Surface, in the Graphics window toolbar, click next
to View Unhidden, then choose View All.

ADD MULTIPHYSICS
1 In the Physics toolbar, click Add Multiphysics to open the Add Multiphysics window.
2 Go to the Add Multiphysics window.
3 In the tree, select No Predefined Multiphysics Available for the Selected Physics Interfaces.
4 Find the Select the physics interfaces you want to couple subsection. In the table, clear
the Couple checkbox for Laminar Flow (spf).
5 In the tree, select Heat Transfer > Radiation > Heat Transfer with Surface-to-
Surface Radiation.
6 Click the Add to Component button in the window toolbar.
7 In the Physics toolbar, click Add Multiphysics to close the Add Multiphysics window.

24 | ELECTRONIC CHIP COOLING

MULTIPHYSICS

Heat Transfer with Surface-to-Surface Radiation 1 (htrad1)

In the Settings window for Heat Transfer with Surface-to-Surface Radiation, in the Graphics
window toolbar, click next to View Unhidden, then choose View Unhidden.

MATERIALS

Heat sink walls

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

Channel walls
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 In the Graphics window toolbar, click next to View Unhidden, then choose
View All.
5 Select Boundaries 1, 3, 4, and 44 only.
6 In the Graphics window toolbar, click next to View Unhidden, then choose
View Unhidden.
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. And just before, edit the first study to exclude

25 | ELECTRONIC CHIP COOLING

 surface-to-surface to make sure the same solution will be computed in case it is solved
again.

STUDY 1 WITHOUT RADIATION

1 In the Model Builder window, click Study 1.
2 In the Settings window for Study, type Study 1 Without Radiation in the Label text
field.

Step 1: Stationary
1 In the Model Builder window, under Study 1 Without Radiation click Step 1: Stationary.
2 In the Settings window for Stationary, locate the Physics and Variables Selection section.
3 In the Solve for column of the table, under Component 1 (comp1), clear the checkbox for
Surface-to-Surface Radiation (rad).
4 In the Solve for column of the table, under Component 1 (comp1) > Multiphysics, clear
the checkbox for Heat Transfer with Surface-to-Surface Radiation 1 (htrad1).

ADD STUDY
1 In the Study toolbar, click Add Study to open the Add Study window.
2 Go to the Add Study window.
3 Find the Studies subsection. In the Select Study tree, select General Studies > Stationary.
4 Right-click and choose Add Study.
5 In the Study toolbar, click Add Study to close the Add Study window.

STUDY 2 WITH RADIATION

1 In the Settings window for Study, type Study 2 With Radiation in the Label text field.
2 In the Study toolbar, click Compute.

RESULTS

Transparency 1
1 In the Model Builder window, expand the Temperature (ht) 1 node.
2 Right-click Volume 1 and choose Transparency.

RESULTS

Solid Temperature
In the Model Builder window, expand the Results > Temperature and Fluid Flow (nitf1) 1
node.

26 | ELECTRONIC CHIP COOLING

Filter 1
1 In the Model Builder window, expand the Results > Temperature and Fluid Flow (nitf1) 1
> Fluid Flow node, then click Filter 1.
2 In the Settings window for Filter, locate the Element Selection section.
3 In the Logical expression for inclusion text field, type spf.U>1.2*nitf1.Uave.
4 In the Temperature and Fluid Flow (nitf1) 1 toolbar, click Plot.

Temperature of the channel walls and heat sink, with radiation

1 In the Model Builder window, right-click Temperature and Fluid Flow (nitf1) 1 and
choose Duplicate.
2 In the Settings window for 3D Plot Group, type Temperature of the channel walls
and heat sink, with radiation in the Label text field.

3 Locate the Color Legend section. Clear the Show units checkbox.

Fluid Flow
1 In the Model Builder window, expand the Temperature of the channel walls and heat sink,
with radiation node.
2 Right-click Fluid Flow and choose Delete.

Temperature of the channel walls and heat sink, with radiation

1 In the Model Builder window, under Results click
Temperature of the channel walls and heat sink, with radiation.

27 | ELECTRONIC CHIP COOLING

2 In the Temperature of the channel walls and heat sink, with radiation toolbar, click
Plot.

By comparing this plot with the previous temperature plot 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.
In order to visualize the temperature on each side of the thermal contact, follow the next
steps.

RESULT TEMPLATES
1 In the Results toolbar, click Result Templates to open the Result Templates window.
2 Go to the Result Templates window.
3 In the tree, select Study 2 With Radiation/Solution 2 (sol2) >
Heat Transfer in Solids and Fluids > Contact Temperature (ht).
4 Click the Add Result Template button in the window toolbar.
5 In the Results toolbar, click Result Templates to close the Result Templates window.

28 | ELECTRONIC CHIP COOLING

RESULTS

Surface Slit 1
1 In the Model Builder window, expand the Results > Contact Temperature (ht) node, then
click Surface Slit 1.
2 In the Contact Temperature (ht) toolbar, click Plot.

29 | ELECTRONIC CHIP COOLING

30 | ELECTRONIC CHIP COOLING