IPC-7351-2005_表面贴装焊盘布局设计和标准通用要求.pdf - 第75页

15.3.2 Carrier Package Format The carrier package for- mat for the SON includes anti-static tubes, since the units have no leads that can bend, as well as conductive carrier tape and reel. 15.3.3 Process Considerations T…

15.2.1 Marking All parts shall be marked with a part

number and ‘‘Pin 1’’ location. ‘‘Pin 1’’ location may be

molded into the plastic body or a chamfer/radius in the

bottom exposed pad (bottom paddle).

15.2.2 Carrier Package Format The carrier package for-

mat for QFN packages include embossed tape and reel as

well as packaging trays.

15.2.3 Process Considerations Because of the small

lead surface area and the sole reliance on printed solder

paste on the PCB surface, the formation of reliable solder

joints for the QFN package can be a challenge. This is fur-

ther complicated by the large thermal pad underneath the

package and its proximity to the inner edges of the leads.

Special considerations are needed in stencil design and

paste printing for both perimeter and thermal pads. Since

surface mount process varies from company to company,

careful process development is recommended.

The optimum and reliable solder joints on the perimeter

pads should have about 50 µm to 75 µm standoff height. A

side ﬁllet is not required since the sides are not designed as

a solderable surface (see IPC-A-610).

15.2.4 Solder Resist Considerations The solder resist

opening should be 120 µm to 150 µm larger than the land

size resulting in 60 µm to 75 µm clearance between the

copper land and solder resist. This allows for solder resist

registration tolerances, which are typically between 50 µm

to 65 µm, depending upon the board fabricators’ capabili-

ties. Typically each land on the PCB should have its own

solder resist opening with a web of solder resist between

two adjacent lands. Since the web has to be at least 75 µm

in width for the solder resist to adhere to the PCB surface,

each land can have its own solder resist opening for lead

pitch of 0.5 mm or higher, based on the land width dimen-

sions. However, for 0.4 mm pitch parts with PCB land

width of 0.25 mm, not enough space is available for solder

resist web in between the land. In such cases, it is recom-

mended to use the ‘‘gang’’ type solder resist opening

shown in Figure 3-22 where a big opening is designed

around all land on each side of the package with no solder

resist in between the land.

15.3 Small Outline No-Lead (SON) The Small Outline

No-lead Package (SON) is a rectangular semiconductor

package with metal terminals along two sides of the bottom

of the package. The terminals are either ﬂush with the bot-

tom or protruding slightly below the bottom of the pack-

age, with plastic mold compound present on three sides of

each contact. The main body of the component is generally

a molded plastic. The SON package is similar to the leaded

SOIC family, though consuming less of the PCB area in

comparison with the leaded SOIC. The part is a ‘‘lead-

less’’ package design with bottom paddle which can be

soldered to the PCB. See Figure 15-3 for an example of a

SON component.

15.3.1 Marking All parts shall be marked with a part

number and ‘‘Pin 1’’ location. ‘‘Pin 1’’ location may be

molded into the plastic body or a chamfer/radius in the

bottom exposed pad (bottom paddle).

IPC-7351-15-02

Figure 15-2 Quad Flat No-Lead (QFN) Construction (Cross-Sectional View)

IPC-7351-15-03

Figure 15-3 Small Outline No-Lead (SON) Construction

IPC-7351 February 2005

标准分享网 www.bzfxw.com 免费下载

15.3.2 Carrier Package Format The carrier package for-

mat for the SON includes anti-static tubes, since the units

have no leads that can bend, as well as conductive carrier

tape and reel.

15.3.3 Process Considerations The SON package is

resistant to failure from board bending (ﬂexing); it features

a metal bottom paddle, which can be soldered directly to

the PC board. This adds adhesive strength while avoiding

messy epoxy under-ﬁll. Though not required, it is highly

recommended that this bottom paddle be soldered to the

printed board, especially for printed boards with signiﬁcant

ﬂex. For the more ﬂex-resistent printed boards, the bottom

paddle soldering is not necessary but is recommended due

to CTE stresses and possible ground signals through the

bottom paddle.

15.3.4 Solder Resist Considerations The solder resist

opening should be 120 µm to 150 µm larger than the land

size resulting in 60 µm to 75 µm clearance between the

copper land and solder resist. This allows for solder resist

registration tolerances, which are typically between 50 µm

to 65 µm, depending upon the board fabricators’ capabili-

ties. Typically each land on the PCB should have its own

solder resist opening with a web of solder resist between

two adjacent lands. Since the web has to be at least 75 µm

in width for solder resist to adhere to the PCB surface, each

land can have its own solder resist opening for lead pitch

of 0.5 mm or higher, based on the land width dimensions.

However, for 0.4 mm pitch parts with PCB land width of

0.25 mm, not enough space is available for solder resist

web in between the land. In such cases, it is recommended

to use the ‘‘gang’’ type solder resist opening shown in

Figure 3-22 where a big opening is designed around all

land on each side of the package with no solder resist in

between the land.

16 ZERO COMPONENT ORIENTATIONS

The zero component orientations expressed in IPC-7351

are deﬁned in terms of the standard component CAD

library with respect to a given PCB design. Recognizing

that a single land pattern may be used for the same compo-

nent part from different suppliers and that each component

supplier may have different orientations on their reels or

that the components may come in trays, there exists the

possibility that the PCB designer loses the ability to refer-

ence a single land pattern if the zero rotation of a part is

according to the method the component is delivered to the

assembly machine. Since the CAD library contains a single

land pattern, the zero component rotation is thus deﬁned

according to the CAD library. Subsequently, component

suppliers can identify the orientation of the parts on the

reels by associating the placement of the part on the reel to

zero orientations deﬁned in IPC-7351. If pin 1 is at the

lower left as deﬁned by the pick and place machine tape

and reel, for example, then the component on the reel is

rotated 90° counterclockwise from the zero rotation given

in IPC-7351. Standardizing the orientation of components

for the installation and utilization of various packaging

methods, such as tubes, trays or tapes and reels, among the

variations of automated assembly equipment existing today

is outside the scope of this document.

Figure 16-1 lists the most commonly used parts and their

proper zero component rotation.

February 2005 IPC-7351

Package Outline Component Examples

Zero Rotation

Pin 1 on Left Side

Land Pattern

Note: Pin 1 is always

the ''Positive Pin''

Chip

Components

Chip Capacitor

Chip Resistor Chip Inductor

Molded

Capacitors

Pin 1 on Left Side

Land Pattern

Note: Pin 1 is always

the ''Positive Pin''

Pin 1 on Left Side

Land Pattern

Note: Pin 1 is always

the ''Positive Pin''

Precision Wire

Wound

Components

Pin 1 on Left Side

Land Pattern

Note: Pin 1 is

always the

Cathode

MELF

Diodes

Molded

Inductors

Pin 1 on Left Side

Land Pattern

Note: Pin 1 is always

the ''Positive Pin''

Molded

Diodes

Pin 1 on Left Side

Land Pattern

Note: Pin 1 is always

the Cathode

Figure 16-1 Zero Component Rotations for Common Package Outlines

IPC-7351 February 2005

标准分享网 www.bzfxw.com 免费下载