General
hardware design/BGA PCB design

From Texas Instruments Wiki

< General
hardware design

Jump to: navigation,
search

Contents

1 BGA PCB Design Main
Page

1.1 BGA Ball Pad
Size

1.2 PCB Routing
Methods

1.2.1 What is Via
Channel(TM)?

1.2.2 PCB Feature Sizes For
Standard BGAs

1.2.3 PCB Layer Count For
Standard BGAs

1.2.4 PCB Feature
sizes for Via Channel(TM) BGAs

1.2.5 PCB Layer Count
For Via Channel(TM) BGAs

1.3 BGA Decoupling
(Bypass) Capacitor Selection and Placement

1.4 Other good BGA
Information

1.4.1 Suggested BGA Solder
Temperature Profile

1.4.1.1 BGA PCB feature
definitions (for the purposes of this page)

1.4.1.2 Conversion
between mm and mils

BGA PCB Design Main
Page

This page is designed to help customers understand what's involved with PCB
design for BGAs.  There is a "definitions" section at the end of this page
for those who may not know all the terms used here.

For the special page on 0.65mm pitch routing, click below.

0.65mm
pitch BGA Special Considerations

BGA Ball Pad
Size

One of the most common questions we get is about what ball pad size to
use.  Optimal BGA ball pad size is easily found by referencing the IPC.org
specifications for ball pad sizing.  The IPC is an organization that is
made up of hundreds of PCB manufacturers and assemblers worldwide working
together to determine the optimal specifications for high PCB yield and
reliability including BGA ball pads.

The IPC has a specification called IPC-7351A.  This specification
provides recommendations for all known BGA ball
sizes.  Referencing this table will show the optimal ball pad size for
any BGA design:

IPC-7351A for NSMD Pads

Nominal

Ball

Diameter*

Reduction

Land

Pattern

Density Level

Nominal

Land

Diameter

Land

Variation

0.75

25%

A

0.55

0.60-0.50

0.65

25%

A

0.50

0.55-0.45

0.6

25%

A

0.45

0.50-0.40

0.55

25%

A

0.40

0.45-0.35

0.5

20%

B

0.40

0.45-0.35

0.45

20%

B

0.35

0.40-0.30

0.4

20%

B

0.30

0.35-0.25

0.35

20%

B

0.30

0.35-0.25

0.3

20%

B

0.25

0.25-0.20

0.25

20%

B

0.20

0.20-0.17

0.2

15%

C

0.17

0.20-0.14

0.17

15%

C

0.15

0.18-0.12

0.15

15%

C

0.13

0.15-0.10

Can be found on the TI Mechanical package drawing available in the
TI product folder.

This table is very handy.  If someone wanted to look up the correct pad
size for a 0.8mm pitch BGA, they can look at the mechanical diagram for that
package to determine the ball size.  For most embedded procesor 0.8mm pitch
BGAs, the ball size is 0.5mm.  Find 0.5mm on the left hand column and
follow that to the column that says "Nominal Land Diameter" and see that the
recommendation for the ball pad is 0.4mm.

The far left column shows acceptable manufacturing variances, not
allowable design targets (all manufacturing has tolerances), so please use the
"Nominal Land Diameter" column to determine the correct BGA ball pad design
target size.

PCB Routing
Methods

Types of arrays:

For embedded processors, TI makes two types of BGAs

1.  Standard BGA arrays.  These are characterized by the standard
footprint which is usually either a full array (fully populated), or an array
with a "moat" (a square of depopulated balls in the array that separates the
inner array, which is mostly power and ground balls, with the outer array of
signals).

2.  Via Channel(TM) arrays.  These are BGA arrays that have
sections of depopulated balls and when viewed from a distance look like an
explosion, or snowflake pattern.  These arrays are specifically
designed to reduce PCB cost by allowing large PCB feature sizes and reduced
PCB layers.  If a part uses a Via Channel BGA array, it is mentioned on the
bulleted list on the first few pages of the part data sheet and there
should be a PCB layout application note like the OMAP 3530 note at the end of
this page.  Only TI makes Via Channel parts.

What is Via
Channel(TM)?

Via Channel is a new TI feature specifically designed to reduce PCB
manufacturing cost by placing the BGA balls in patterns specifically
designed for optimal via and trace placement.

This feature uses a special BGA array design to allow two major
advantages:

- Large PCB feature sizes (regardless of ball pitch)

- Reduced PCB layer count (because of the increased layer efficiency)

Currently there are five main embedded processor product lines with a Via
Channel package, and more are on the way.

Via Channel BGA arrays are designed to use standard PCB processes
(no micro vias or HDI required) regardless of ball pitch, and they have
much reduced PCB layer requirements.  All current Via Channel designs
can be done in 4 total PCB layers (see the Via Channel PCB layer section below).

To learn more about this unique design feature, here's a short slide set to
explain graphically how Via Channel works:

"What
is Via Channel" Presentation

PCB
Feature Sizes For Standard BGAs

Standard arrays are fairly easy to estimate PCB feature sizes and layers
for.  These figures can be arrived at with a calculator, however be careful
to make sure a line of the specified width can be used in between vias of the
specified width.  Just because an 16 mil via can be used on a 0.65mm
pitch part does not mean it's possible to route a 4 mil trace in between the
vias.

PCB Typical Feature Sizes For Standard (non-Via Channel) BGA Arrays

Ball Pitch

Via Diameter

Via Hole

Size

Trace Size

Clearance

Micro

Vias?

0.8mm pitch

18 mil

10-8 mil

4-5 mil

4 mil

No

0.65mm pitch

16 mil*

12 mil

8 mil*

6 mil

4 mil*

4 mil

4 mil*

4 mil

No

Yes

0.5mm pitch

10 mil

5 mil

3 mil

3 mil

Yes

0.4mm pitch

10-8 mil

5-4 mil

3 mil

3 mil

Yes

16 mil diameter/8 mil hole vias are only possible if done in a creative
way that puts traces only in between every other via.  In other words,
16/8 vias, when placed between the balls, will move enough to allow one 4 mil
trace per pair, but not one 4 mil trace per via, so for some designs like the
DM365 and DM355, 16/8 mil vias should be possible in your application since
there are some areas to place vias in the array.  However for Freon,
since it's a full array, it is not possible to use 16/8 vias unless only every
other pin is used (not likely).  16/8 vias are uncommon in the
PCB fab world, but some companies can do them without micro vias.

PCB Layer
Count For Standard BGAs

The layers required to route a particular design can be easily estimated once
the signals and location of those signals has been highlighted.

Assuming that the above required PCB feature sizes for that
pitch are used, the PCB layers will be used as follows:

The first 2 rows will route on the top layer

The second 2 rows will route on the second layer

An additional PCB layer will be required for every row in past the first
4.

So, if "Rows_in" = the maximum number of rows in (from the outside of the BGA
array) the centermost signal is located, then:

2 Rows_in = 1 PCB signal layer

3 Rows_in = 2 PCB signal layers

4 Rows_in = 2 PCB signal layers

5 Rows_in = 3 PCB signal layers

6 Rows_in = 4 PCB signal layers

7 Rows_in = 5 PCB signal layers

So if a signal called I2C_CLK was required in the design, and it was located
five rows in from the outside (counting all rows), then it would require 3 PCB
signal layers, plus at least 2 PCB layers for power and ground, so that's 5
PCB layers total, which makes a 6 layer board (it doesn't make sense to build an
odd layer board).

PCB Feature
sizes for Via Channel(TM) BGAs

If the part used is a Via Channel(TM) part, it has been specifically designed
to reduce PCB costs.  The PCB feature sizes are now independant of the ball
pitch since the vias no longer have to be placed in between four balls.
Via Channel also routes more signals out on lower layers.  Where standard
array trace density on lower PCB layers is limited by via interference of the
traces, Via Channel designs are mostly free of this restriction, so more traces
can be routed on lower layers thereby reducing the number of PCB layers
required.  Most Via Channel designs are designed for a four layer PCB
(minimum).

PCB Typical Feature Sizes For Via Channel BGA Arrays

Ball Pitch

Via Diameter

Via Hole

Size

Trace Size

Clearance

Micro

Vias?

0.8mm pitch

20 mil

18 mil

12-10 mil

10-8 mil

5 mil

4 mil

5 mil

4 mil

No

0.65mm pitch

20 mil

18 mill

12-10 mil

10-8 mil

4 mil

4 mil

4 mil

4 mil

No

No

0.5mm pitch

18 mil

10 mil

4 mil

4 mil

No

PCB
Layer Count For Via Channel(TM) BGAs

Via Channel BGAs are specifically designed to require only 4 total PCB
layers.  Depending on the power requirements and the power signal
routing, an additional power layer may be required bringing the PCB layers to 6,
but with very careful design this should be able to be avoided.

BGA
Decoupling (Bypass) Capacitor Selection and Placement

BGA
Decoupling Capacitor Selection and Placement

Other good BGA
Information

Some good TI application notes on BGAs:

CUS
package (OMAP 3530) Via Channel BGA routing application note

More to come

Suggested BGA Solder Temperature
Profile

under construction

BGA
PCB feature definitions (for the purposes of this page)

Ball pads - Also known as BGA "lands". This is the copper that the BGA
ball solders to.

NSMD pad - Non-Solder Mask Defined ball pad. This kind of pad has an
opening that is defined only by the size of the ball pad. The solder mask is
applied around the ball pad and does not cover it. This kind of pad is more
popular lately and has the advantage of increased ball adhesion because the
ball flows around the sides of the ball pad and grips on the top and the
sides. This kind of pad is usually recommended for BGA designs 0.5mm and
above.

SMD pad - Solder Mask Defined ball pad. This kind of pad has a large
copper area, but the solder mask covers the edges, so the opening is known as
solder mask defined. This kind of pad is sometimes best for very small pitch
pads where ball shorting is an issue.

Via diameter - the full width of the via annular ring

Micro via - a via that is laser drilled.

HDI - High Density Interconnect. This is the type of board that uses very
small vias like micro vias. When a board uses micro vias it is called an HDI
board.

Conversion
between mm and mils

• 0.075mm = 3 mils (0.003”)
• 0.1mm = 4 mils (0.004”)
• 0.125mm = 5
mils (0.005”)
• 0.2mm = 8 mils (0.008”)
• 0.4mm = 16 mils (0.016”)
•
0.45mm = 18 mils (0.018”)
• 0.5mm = 20 mils (0.020”)

For technical support please post your questions at http://e2e.ti.com/. Please
post only comments about the article General hardware design/BGA PCB
design here.

Links

Amplifiers & Linear
Audio
Broadband RF/IF & Digital Radio
Clocks & Timers
Data Converters

DLP & MEMS
High-Reliability
Interface
Logic
Power Management

Processors

ARM Processors

Digital Signal Processors (DSP)

Microcontrollers (MCU)

OMAP Applications Processors

Switches & Multiplexers
Temperature
Sensors & Control ICs
Wireless Connectivity

Retrieved from "http://processors.wiki.ti.com/index.php?title=General_hardware_design/BGA_PCB_design&oldid=102606"

Category:

Schematic
Checklists

Navigation menu

Personal tools

Create
account

Log
in

Namespaces

Page

Discussion

Variants

Views

Read

View
source

View
history

More

Search

Navigation

Main
Page

All
pages

All
categories

Recent
changes

Random
page

Help

Print/export

Create
a book

Download
as PDF

Printable
version

Toolbox

What
links here

Related
changes

Special
pages

Permanent
link

Page
information

This page was last modified on 30 March 2012, at
15:21.

This page has been accessed 866 times.

Content is available under Creative
Commons Attribution-ShareAlike unless otherwise noted.

Privacy
policy

About
Texas Instruments Wiki

Disclaimers