Fairchild Semiconductor
Application Note
January 2001
Revised September 2001
Using BGA Packages
TABLE 1. BGA Space Savings
Compared to Surface Mount Packages
Demanding space and weight requirements of personal
computing and portable electronic equipment has led to
many innovations in IC packaging. Combining the right
interface and logic products with new package technology
can have a significant impact on the capabilities and formfactor of the end product. Leaded surface mount devices
are constantly pushing the manufacturing capabilities of
leading board manufacturers to finer and finer lead pitch
geometry’s to increase I/O density and reduce board
of Bits
36 to 48
> 66%
> 47%
> 59%
32 to 40
> 67%
18 to 24
16 to 20
This requirement has lead to significant interest in the
JEDEC (Joint Electron Device Engineering Council) registered Fine-Pitch Ball Grid Array (FBGA) package. These
packages are ideally suited to low cost, high volume applications, where package size and performance is of major
importance. Typical BGA applications include:
1. Notebook computers
2. Personal Digital Assistants (PDA’s)
3. Mobile telephone handsets
4. High density disk drives
5. Camcorders
6. Digital cameras
BGA advantages compared to fine pitch QFP or TSSOP
1. BGAs are usually smaller.
2. BGAs have larger pitch.
3. BGAs have no fragile leads, that causes yield and
rework problems.
4. Board assembly yields are significantly improved.
5. Board inspection can be reduced.
6. BGAs have better thermal and electrical properties.
7. In many applications, the use of BGA results in significant system level cost savings.
FIGURE 1. 114 Ball BGA vs. Surface Mount
Surface Mount vs. BGA
At 0.4 to 0.5mm pin pitch, the race to finer surface mount
lead pitches has hit several technical and economic walls.
Manufacturing anything smaller will significantly impact
PCB yield and push board costs above acceptable levels
for the highly competitive and cost conscious electronics
industry. Avoiding problems such as bent leads and solder
bridging become significant manufacturing challenges.
Additionally, electrical problems such as crosstalk become
a major issue due to the length and close pitch of the leads
on surface mount packages.
Alternatively, BGA packaging uses relatively wide “pad to
pad” pitch rules and when coupled with existing PCB manufacturing processes result in high yields. The “array”
approach improves I/O density and reduces the board
space consumed by the device. Table 1 and Figure 1 show
examples of space savings of BGA over surface mount
© 2001 Fairchild Semiconductor Corporation
AN-5026 Using BGA Packages
BGA Routing
Fairchild Semiconductor BGA products are all designed around the JEDEC standard 0.8mm ball pitch and large 0.5mm ball
size. This allows for economical 0.15mm (6 mil) line and space PCB manufacturing processes as well as optimized reliability. Figure 2 shows two 0.15mm (6 mil) line routing techniques.
FIGURE 2. BGA Routing
Figure 3 through Figure 7 illustrate the basic routing techniques of the different bit-count devices.
FIGURE 3. 54-Ball 18-Bit BGA Routing (74LCX16500)
FIGURE 4. 54-Ball 24-Bit BGA Routing (FST16211)
FIGURE 5. 96-Ball 32-Bit BGA Routing (74VCX32374)
Note: Various techniques for routing internal control pins.
BGA Routing
FIGURE 6. 114-Ball 36-Bit BGA Routing (74VCX32500)
FIGURE 7. 114-Ball 40-Bit BGA Routing (FST32211)
Note: The FST32211 can also be routed as a 43-bit switch without the use of vias.
Routing Power and Ground:
Power and ground balls have not been routed in the illustrations above because of the designers multiple routing
choices. There are generally two methods:
2. Supplying power and ground to the BGA by connecting
vias to the VCC/GND plains and traces outside the BGA
package. See Figure 9.
1. Supplying power and ground to the BGA by connecting
vias to the VCC/GND planes and traces under the BGA
package. See Figure 8 for via placement.
Pros: Allows for larger vias outside the package.
Cons: Compromised noise performance through trace
length added VCC/GND trace length.
Pros: Better noise performance due to lower power
inductance (shorter VCC/GND trace length).
Cons: Via size under the package is restricted to
0.56mm (22.0 mil) vias.
FIGURE 8. BGA Powered
Vias Under the Package
FIGURE 9. BGA Powered
Vias Outside the Package Land Area
BGA Via Design and Layout Options
When using vias in high bit-count devices such as the 48-bit FST32211 (see Figure 10), via density and placement become
critical issues for the layout designer. The use of through-board vias allows access to all signal bits on the device; this helps
contribute to maximum space integration. Additionally, the board backside vias can be used to connect components such
as termination and decoupling devices if needed.
FIGURE 10. 114-Ball 48-Bit BGA with Vias (FST32211)
Note: For a via free 48-bit bus switch solution two FST16211
can be used with a minimal loss in space savings. (see Figure 4)
Figure 11 shows ball pads to via spacing with a BGA 0.8mm pitch and a 0.56mm via, which give a 0.11mm via to ball spacing. Figure 12 shows a board cross-section with non-solder mask defined pads-to-via spacing dimensions. Manufacturing
technology and expense are the deciding factors in via size. Larger vias allow for more relaxed manufacturing rules and
lower costs. Smaller vias are more costly due to the high end manufacturing equipment and higher drill bit breakage.
FIGURE 11. BGA Via to Ball Spacing Diagram
FIGURE 12. Board with Non-Solder Mask Defined Pads to Via Spacing
Micro vias are very small vias (4µm is typical) and can be
used for via in pad layouts. This can significantly reduce via
density, increase routing options on the board, and conserve space. Laser technology is often used to drill micro
vias. Lasers drill micro vias through a 4 millimeter thick
dielectric layer, allowing connection to the first internal
layer of the board. Two 4 millimeter layers can be drilled
with a laser, allowing connection from the surface to the
second board layer.
Through-board vias are the most economical via type from
a board manufacturing perspective. However, trade-offs in
highly space-constrained designs may be required.
Through-board vias create a matrix of vias on the board
backside, limiting its use for traces and components. These
vias can also disrupt the smooth layout of bus runs on
internal board layers or limit their placement.
With the ever increasing demand for more compact systems and higher density layouts, three more advanced
methods of via connections are being used, the blind via,
the buried via, and the micro via. Figure 13 shows an
example of these via types used in conjunction with a BGA.
These three via types are more costly than through-board
vias from a manufacturing standpoint. However, there are
two significant advantages over through-board vias; the
elimination of backside vias frees that layer for component
placement, and some internal layers and the backside are
freed up for traces and uninterrupted bus runs.
Blind vias connect one side of the board to some inner layers, but do not run completely through to the other side.
Buried vias connect internal board layers but do not extend
to the exterior of the board.
FIGURE 13. Multi Layer Board with BGA Connections to Micro Vias, Buried Vias and Blind Vias
BGA Via Design and Layout Options
BGA Board Design
BGA Mounting Process
To achieve maximum reliability, the design of the PCB on
which the BGA is mounted should be considered. In particular, the diameter of package lands and board lands are
very important. The actual sizes of these dimensions are
key factors, but their ratio is also of critical importance. Figure 14 shows a BGA Board Layout with the optimum 1 to 1
ratio for package land to PCB land. This optimized ratio
equalizes stresses, reducing the chances of a stress
cracked solder ball, which will lead to premature system
failure. Ratios other than 1 to 1 will lead to unequal distribution of stress loads. For example, solder lands that are
larger than the package lands will place a greater amount
of stress on the ball at the package land to ball interface.
This can cause cracking and premature failure at the package land to ball interface.
Replacing leaded packages with BGA’s offers several
board assembly advantages:
1. Improved device planarity
2. No chance to bend leads
3. Greater pad to pad spacing
With no chance to bend or deform leads, BGA products
offer PCB manufacturers a significant yield improvement
over similar lead count fine-pitch surface mount devices.
Another important feature of BGA products is their ability to
self-align over the PCB solder lands.
This feature is caused by the surface tension of the solder
balls pulling the BGA over the pads.
The use of solder paste is recommended for mounting
BGA devices, although it is possible to omit the paste, and
only use a flux. The advantages of using paste are:
1. Paste acts as a flux, and aids wetting of the solder ball
to the PCB land.
2. Paste, being sticky, helps hold the component in place
during reflow.
3. Paste helps to overcome any minor variations in planarity of the solder balls.
4. Paste contributes to the final volume of solder in the
joint, and thus allows this volume to be varied to give
an optimum joint.
FIGURE 14. BGA Board Layout
A = Land diameter on package
B = Land diameter on printed circuit board
No-clean type pastes are recommended, due to difficulty in
cleaning under the mounted component.
Ratio A/B = 1 for best case reliability
In order to produce the optimum solder joint, it is important
to understand the amount of collapse of the solder balls,
and the overall shape of the joint. These are a function of:
1. The diameter of the BGA solder ball vias.
In practice optimum land diameters are as follows:
Solder Mask defined pads:
2. The volume and type of solder paste screened onto the
3. The diameter of the PCB land.
Non-Solder Mask defined pads: 0.350mm
4. The board assembly re-flow conditions.
5. The weight of the package.
Experience has shown that solder lands can be either solder mask defined, or non-solder mask defined. However,
non-solder mask defined designs provide additional
ball-to-land contact area, making them the favored option.
The additional contact area is created from the solder ball
to pad side connection made during the soldering process.
As shown in Figure 15 this creates an improved mechanical connection.
As shown in Figure 16, the original ball height on the package is 0.40mm. The ball height typically drops to 0.35mm
after the package is mounted.
FIGURE 16. BGA Solder Ball Collapse
FIGURE 15. Cross-section Comparison of
Solder Mask Defined Pad (left) to
Non-Solder Mask Defined Pad (right)
with BGA Solder Ball Connections
Each of the methods offers advantages and disadvantages. The prototype socket gives the designer the ability
to test multiple devices in the socketed connection. The via
fan-out method, as shown in Figure 17, incorporates a
mounted BGA routed through an array of vias for signal
During the prototype and engineering debug phase it may
be necessary to access IC signals for testing purposes.
Several options exist depending on the specific needs of
the system being developed.
1. Prototype socket for the BGA
2. Via fanout
3. PCB solder mask defined lands
With form factor boards large via arrays remove all the board real estate advantage gained with the BGA packaging. Limited I/O access can still be gained using test points like those shown in Figure 18.
Minimum Size Via Defined Pattern for Prototype Testing
• 19 x 6 ARRAY 0.8mm pitch with package dimensions of 16.0mm x 5.5mm
• Overall dimensions (including TestVia's) 20.1mm x 8.8mm
• 22mil vias, 15mil holes; 6mil line and space PCB rules
FIGURE 17. Via Fan-out for Prototype Testing
Solder Mask Defined Land Pattern for In-System Testing
FIGURE 18. BGA In-System Testing
BGA Testing
AN-5026 Using BGA Packages
Notebook Docking Application
Routing the BGA into the hole pattern created by a typical 0.8mm docking connector can be achieved on a single PCB signal layer. By limiting the signal routing to a single layer, few if any vias are needed for the BGA. Eliminating all datapath vias
allows for greater levels of backside usability and backside component placement.
FIGURE 19. BGA Docking Application
ability. Continued innovations and cost reductions in PCB
manufacturing technology will usher in advances in PCB
design and further the usability and cost effectiveness of
BGA's. With BGA packages already on par with leaded
packages in cost per bit for large-scale designs, and the
continued drive toward system size reduction, FBGA's of
all types are the wave of the future and will soon be everywhere.
FBGA’s offer dramatic new levels of PCB layout and design
possibilities. BGA's offer space savings of 60% or more vs.
TSSOP and greater than 37% over comparable TVSOP
and QVSOP packaging. By understanding how to effectively use these new packages, PCB and system designers
can create electronic systems with greater component density, miniaturization and functionality. An additional benefit
is system manufacturing with less re-work and more reli-
Fairchild does not assume any responsibility for use of any circuitry described, no circuit patent licenses are implied and
Fairchild reserves the right at any time without notice to change said circuitry and specifications.
2. A critical component in any component of a life support
device or system whose failure to perform can be reasonably expected to cause the failure of the life support
device or system, or to affect its safety or effectiveness.
1. Life support devices or systems are devices or systems
which, (a) are intended for surgical implant into the
body, or (b) support or sustain life, and (c) whose failure
to perform when properly used in accordance with
instructions for use provided in the labeling, can be reasonably expected to result in a significant injury to the