PDF
Convection Cooling of Circuit Boards — 3D Forced Convection
Introduction
This example models the air cooling of circuit boards populated with multiple integrated circuits (ICs), which act as heat sources. Two possible cooling scenarios are shown in Figure 1: vertically aligned boards using natural convection, and horizontal boards with forced convection (fan cooling). In this case, contributions caused by the induced (forced) flow of air dominate the cooling. To achieve high accuracy, the simulation models heat transport in combination with the fluid flow.
Figure 1: Stacked circuit boards with multiple in-line heat sources. Line A represents the centerline of the row of ICs, and the area between lines A–B on the board represents the symmetry.
A common technique is to describe convective heat flux with a film-resistance coefficient, h. The heat-transfer equations then become simple to solve. However, this simplification requires that the coefficient is well determined which is difficult for many systems and conditions.
An alternative way to thoroughly describe the convective heat transfer is to model the heat transfer in combination with the fluid-flow field. The results then accurately describe the heat transport and temperature changes. From such simulations it is also possible to derive accurate estimations of the film coefficients. Such models are somewhat more complex but they are useful for unusual geometries and complex flows. The following example models the heat transfer of a circuit-board assembly using the Conjugate Heat Transfer predefined multiphysics coupling of the Heat Transfer Module. The modeled scenario is based on work published by A. Ortega (Ref. 1).
FR4 circuit board material (Ref. 2) and silicon are used as the solid materials composing the circuit board system. The model treats air properties as temperature dependent.
The dimensions of the original geometry are:
•
Board: length (in the flow direction) is 130 mm, and thickness is 2 mm
•
ICs: length and width are both 20 mm, and thickness is 2 mm
•
The boards are spaced 10 mm apart
Model Definition
This example simulates the horizontal board with forced convection cooling as shown on the right side of the Figure 1. Due to symmetry, it is sufficient to model a unit cell, from the back side of a board to the next back side, covering the area between lines A and B. Figure 2 depicts the three-dimensional geometry.
Figure 2: The modeled geometry in 3D.
The model makes use of the Conjugate Heat Transfer predefined multiphysics coupling with a stationary study to set up the simulation. The heat rate per unit volume is 1.25 MW/m3. To model forced convection, set up an inlet-velocity profile, uy, that is uniform in the (horizontal) x direction and parabolic (similar to a fully developed laminar profile) in the (vertical) z direction. In terms of an equation this reads
where z’ = z ⁄(10 mm) parameterizes the height above the board and umax, the maximal inlet speed, equals 1 m/s. At the outlet, all the models use a zero pressure boundary condition. In addition, no slip conditions at the surfaces of the board and the ICs are applied. Periodic conditions are used on the board surfaces to model the other boards in the stack. Finally, the models apply continuity of temperature and heat flux at all interior boundaries.
Results and Discussion
In this example, a forced fluid inlet velocity represents the situation when a fan cools the ICs. Figure 3 shows the resulting temperature distribution. The temperature rise in the ICs is approximately 20–35 K smaller compared to that for natural-convection case (see Convection Cooling of Circuit Boards — 3D Natural Convection for the model description and results). This is due to the higher average fluid velocity. In the forced convection case, the temperature difference along the board is also less pronounced than for the natural convection.
Figure 3: Temperature distribution in the case of forced convection cooling of horizontal boards.
Another interesting result, visible in Figure 4, is that the channeling effect of the gap causes a reduction of the fluid’s velocity at the very surface of the sources. The cooling of the ICs is therefore somewhat reduced compared to an ideal case with an even flow field.
Figure 4: Velocity distribution for the case of forced convection.
The symmetry conditions used in the model indicate that the model accounts for multiple chips and boards corresponding to the boards configuration shown in Figure 1. Figure 5 shows the temperature profile on the stacked circuit boards and the streamlines in the surrounding air.
Figure 5: Temperature profile on the stacked circuit boards and streamlines.
References
1. A. Ortega, “Air Cooling of Electronics: A Personal Perspective 1981-2001,” presentation material, IEEE SMITHERM Symposium, 2002.
2. C. Bailey, “Modeling the Effect of Temperature on Product Reliability,” Proc. 19th IEEE SMITHERM Symposium, 2003.
Application Library path: Heat_Transfer_Module/Power_Electronics_and_Electronic_Cooling/circuit_board_forced_3d
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 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
In the table, enter the following settings:
Name
Expression
Value
Description
q_source
1[W]/(20*20*2[mm^3])
1.25E6 W/m³
Heating power per unit volume
T0
300[K]
300 K
External air temperature
patm
1[atm]
1.0133E5 Pa
Air pressure
umax
1[m/s]
1 m/s
Inlet velocity
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
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 15.
4
In the Depth text field, type 130.
5
In the Height text field, type 12.
6
Locate the Position section. In the z text field, type -2.
7
Click to expand the Layers section. In the table, enter the following settings:
Layer name
Thickness (mm)
Layer 1
2
8
In the Geometry toolbar, click  Build All.
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 10.
4
In the Depth text field, type 20.
5
In the Height text field, type 2.
6
Locate the Position section. In the y text field, type 10.
7
In the Geometry toolbar, click  Build All.
Array 1 (arr1)
1
In the Geometry toolbar, click  Transforms and choose Array.
2
Select the object blk2 only.
3
In the Settings window for Array, locate the Size section.
4
In the y size text field, type 4.
5
Locate the Displacement section. In the y text field, type 30.
6
In the Geometry toolbar, click  Build All.
7
Click the  Zoom Extents button in the Graphics toolbar.
Definitions
Create appropriate selections to simplify the model specification.
IC
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type IC in the Label text field.
3
Click the  Wireframe Rendering button in the Graphics toolbar to access the domains to select.
4
Select Domains 3–6 only.
Solid Boundaries
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Solid Boundaries in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Select Boundaries 6–9, 11–14, 16–19, 21–24, 26, 27, and 30–33 only.
For more convenience in selecting these boundaries, you can click the Paste Selection button and paste the above numbers.
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
Click the Add to Component button in the window toolbar.
5
In the tree, select Built-in > Silicon.
6
Click the Add to Component button in the window toolbar.
7
In the tree, select Built-in > FR4 (Circuit Board).
8
Click the Add to Component button in the window toolbar.
9
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
Air (mat1)
1
Select Domain 2 only.
2
In the Settings window for Material, locate the Geometric Entity Selection section.
3
Click  Create Selection.
4
In the Create Selection dialog, type Air in the Selection name text field.
5
Click OK.
Silicon (mat2)
1
In the Model Builder window, click Silicon (mat2).
2
In the Settings window for Material, locate the Geometric Entity Selection section.
3
From the Selection list, choose IC.
FR4 (Circuit Board) (mat3)
1
In the Model Builder window, click FR4 (Circuit Board) (mat3).
2
Select Domain 1 only.
Laminar Flow (spf)
1
In the Model Builder window, under Component 1 (comp1) click Laminar Flow (spf).
2
In the Settings window for Laminar Flow, locate the Domain Selection section.
3
From the Selection list, choose Air.
Symmetry 1
1
In the Physics toolbar, click  Boundaries and choose Symmetry.
2
Select Boundaries 4 and 35 only.
Open Boundary 1
1
In the Physics toolbar, click  Boundaries and choose Open Boundary.
2
Select Boundary 5 only.
Inlet 1
1
In the Physics toolbar, click  Boundaries and choose Inlet.
2
Select Boundary 29 only.
3
In the Settings window for Inlet, locate the Velocity section.
4
Click the Velocity field button.
5
Specify the u0 vector as
0
x
-4e4*umax*z*(0.01[m]-z)[1/m^2]
y
0
z
Heat Transfer in Solids and Fluids (ht)
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.
Initial Values 1
1
In the Model Builder window, click Initial Values 1.
2
In the Settings window for Initial Values, locate the Initial Values section.
3
In the T text field, type T0.
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 IC.
4
Locate the Heat Source section. In the Q0 text field, type q_source.
Open Boundary 1
1
In the Physics toolbar, click  Boundaries and choose Open Boundary.
2
Select Boundary 5 only.
3
In the Settings window for Open Boundary, locate the Upstream Properties section.
4
In the Tustr text field, type T0.
Inflow 1
1
In the Physics toolbar, click  Boundaries and choose Inflow.
2
Select Boundary 29 only.
3
In the Settings window for Inflow, locate the Upstream Properties section.
4
In the Tustr text field, type T0.
Periodic Condition 1
1
In the Physics toolbar, click  Boundaries and choose Periodic Condition.
2
Select Boundaries 3 and 7 only.
Mesh 1
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 Coarse.
4
Click  Build All.
You should now see the following meshed geometry.
Study 1
The model is now ready for solving. Optionally, to avoid a warning message about an ill-conditioned preconditioner increase the factor in error estimate as follows.
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Segregated 1.
4
In the Settings window for Segregated, locate the General section.
5
From the Stabilization and acceleration list, choose Anderson acceleration.
6
In the Study toolbar, click  Compute.
Results
Temperature (ht)
To reproduce Figure 3 do as follows.
Streamline 1
In the Temperature (ht) toolbar, click  Streamline.
Selection 1
1
In the Model Builder window, right-click Volume 1 and choose Selection.
2
Select Domains 1 and 3–6 only.
Streamline 1
1
In the Model Builder window, under Results > Temperature (ht) click Streamline 1.
2
In the Settings window for Streamline, locate the Data section.
3
From the Dataset list, choose Study 1/Solution 1 (sol1).
4
Click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Laminar Flow > Velocity and pressure > u,v,w - Velocity field.
5
Locate the Streamline Positioning section. From the Positioning list, choose Starting-point controlled.
6
From the Entry method list, choose Coordinates.
7
In the x text field, type 1+2*range(0,6).
8
In the y text field, type 130.
9
In the z text field, type 1.6.
10
Locate the Coloring and Style section. Find the Line style subsection. From the Type list, choose Tube.
11
Find the Point style subsection. From the Type list, choose Arrow.
12
Find the Line style subsection. In the Tube radius expression text field, type ht.gradTmag[m^2/K].
The streamlines tube radius would correspond to the magnitude of the temperature gradient.
13
Click to expand the Inherit Style section. From the Plot list, choose Volume 1.
14
In the Temperature (ht) toolbar, click  Plot.
15
Click the  Zoom Extents button in the Graphics toolbar.
Velocity (spf)
The second default plot shows the velocity field, the third one shows the pressure field.
To visualize the velocity field (Figure 4), follow the steps below.
Multislice 1
1
In the Model Builder window, expand the Velocity (spf) node, then click Multislice 1.
2
In the Settings window for Multislice, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Laminar Flow > Velocity and pressure > spf.U - Velocity magnitude - m/s.
3
Locate the Multiplane Data section. Find the y-planes subsection. In the Planes text field, type 8.
4
Find the z-planes subsection. In the Planes text field, type 0.
Velocity (spf)
In the Model Builder window, click Velocity (spf).
Arrow Volume 1
1
In the Velocity (spf) toolbar, click  Arrow Volume.
2
In the Settings window for Arrow Volume, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > 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 y grid points subsection. In the Points text field, type 8.
5
Find the z grid points subsection. In the Points text field, type 5.
6
Locate the Coloring and Style section. From the Color list, choose Black.
7
In the Velocity (spf) toolbar, click  Plot.
To create a plot showing several layers of chips as in Figure 5, follow the instructions below.
Study 1/Solution 1 (2) (sol1)
1
In the Model Builder window, expand the Results > Datasets node.
2
Right-click Results > Datasets > Study 1/Solution 1 (sol1) and choose Duplicate.
Selection
1
In the Results toolbar, click  Attributes and choose Selection.
2
In the Settings window for Selection, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Domain.
4
Select Domains 1 and 3–6 only.
Mirror 3D 1
In the Results toolbar, click  More Datasets and choose Mirror 3D.
Array 3D 1
1
In the Results toolbar, click  More Datasets and choose Array 3D.
2
In the Settings window for Array 3D, locate the Data section.
3
From the Dataset list, choose Mirror 3D 1.
4
Locate the Array Size section. In the x size text field, type 3.
5
In the z size text field, type 3.
6
Locate the Displacement section. From the Method list, choose Manual.
7
In the x text field, type 30.
8
In the z text field, type 12.
Array 3D 1, Mirror 3D 1
1
In the Model Builder window, under Results > Datasets, Ctrl-click to select Mirror 3D 1 and Array 3D 1.
2
Right-click and choose Duplicate.
Mirror 3D 2
1
In the Settings window for Mirror 3D, locate the Data section.
2
From the Dataset list, choose Study 1/Solution 1 (2) (sol1).
Array 3D 2
1
In the Model Builder window, click Array 3D 2.
2
In the Settings window for Array 3D, locate the Data section.
3
From the Dataset list, choose Mirror 3D 2.
Temperature (ht)
1
In the Model Builder window, under Results click Temperature (ht).
2
In the Settings window for 3D Plot Group, locate the Data section.
3
From the Dataset list, choose Array 3D 1.
4
Locate the Plot Settings section. Clear the Plot dataset edges checkbox.
Volume 1
1
In the Model Builder window, click Volume 1.
2
In the Settings window for Volume, locate the Data section.
3
From the Dataset list, choose Array 3D 2.
Slice 1
1
In the Model Builder window, right-click Temperature (ht) and choose Slice.
2
In the Settings window for Slice, click to expand the Title section.
3
From the Title type list, choose None.
4
Locate the Plane Data section. From the Plane list, choose zx-planes.
5
In the Planes text field, type 2.
6
Click to expand the Inherit Style section. From the Plot list, choose Volume 1.
Streamline 1
1
In the Model Builder window, click Streamline 1.
2
In the Settings window for Streamline, locate the Data section.
3
From the Dataset list, choose From parent.
4
Click to expand the Title section. From the Title type list, choose Custom.
5
Find the User subsection. In the Suffix text field, type (m/s).
6
Locate the Streamline Positioning section. In the x text field, type range(-13,12,71) range(-13,12,71) range(-13,12,71).
7
In the z text field, type 6,6,6,6,6,6,6,6,18,18,18,18,18,18,18,18,30,30,30,30,30,30,30,30.
8
Locate the Coloring and Style section. Find the Line style subsection. In the Tube radius expression text field, type 0.4.
9
Select the Radius scale factor checkbox. In the associated text field, type 1.
10
Find the Point style subsection.
11
Select the Number of arrows checkbox. In the associated text field, type 150.
12
Locate the Inherit Style section. From the Plot list, choose None.
Color Expression 1
1
In 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 Component 1 (comp1) > Laminar Flow > Velocity and pressure > spf.U - Velocity magnitude - m/s.
3
In the Temperature (ht) toolbar, click  Plot.