IPC-7095C-2013.pdf - 第66页

should be distinct enough so as not to be confused with any other markings around the land pattern. 6.2 Attachment Sites (Land Patterns and Vias) 6.2.1 Big vs. Small Land and Impact on Routing The diameter of the solder …

Nearly all hot air methods use a nozzle system that ﬁts

down over and/or around the BGA package to heat the sol-

der joints for removal and reﬂow. A component keepout

area of 2.5 mm away from the outer edge of the oven

nozzle is suggested. Including the nozzle size results in a

3.8 mm clearance from the component body. This spacing

around the BGA provides room for the nozzle and reduces

the risk of heating solder joints of adjacent components

above the reﬂow temperature. When using laser for rework,

the keepout area can be reduced to under 1 mm.

After a BGA package has been removed from the board

during repair, the solder lands must be cleaned and new

solder paste or ﬂux applied before a new component can be

placed. If the solder paste or ﬂux is dispensed using manual

methods, or if solder paste is applied using an automated

dispensing system, then there are no special component

keepout areas required. However, many repair systems use

a miniaturized stencil and squeegee to manually apply sol-

der paste either to the lands on the board or onto the balls

of the component. In general, a minimum of 3 mm compo-

nent keepout (i.e., the nominal distance between the body

of the component and the body of the neighboring compo-

nent) is needed so that both the nozzle clearance require-

ment and the mini-stencil requirement can be met when

printing to the lands on the board. The existence of a high

proﬁle neighboring component may require the minimum

distance to be much larger than the stated minimum value.

6.1.3 Global Placement There are no special global

placement requirements for BGA packages. However, it is

recommended that they not be placed near the board cen-

terlines. This reduces the potential of coplanarity problems

associated with the board warping during reﬂow. In addi-

tion, BGA packages should not be placed next to large

through-hole components, as these can stiffen the board

and signiﬁcantly increase localized BGA corner joint

stresses. In some cases, one might want to take advantage

of certain features that might actually help protect the BGA

if the induced strain relative to the BGA corners are

reduced by the stiffness caused by nearby through-hole or

other components. Finally, BGA packages should not be

placed with their diagonals in line with mounting stand-off,

bosses, and screws that support or secure the printed board

assembly, since this can induce levels of stress on the cor-

ner balls, which are more susceptible to damage.

6.1.4 Alignment Legends (Silkscreen, Copper Features,

Pin 1 Identifier)

Alignment features printed on the circuit

board are recommended for BGA packages to verify com-

ponent alignment before and after reﬂow. BGA packages,

especially PBGA, will self-align during reﬂow, even when

placed up to 50% off the lands. As a result, any misalign-

ments are generally one land diameter length or more off.

Alignment features will help verify that the component

placement is sufficiently accurate with visual inspection.

Silkscreen and copper are the two main materials used for

alignment legends. Silkscreen is the most visible material,

but requires the additional process step during board manu-

facturing. Copper alignment legends are created at the

same time all other copper features are created and, there-

fore, lead to more accurate placement. Higher speed cir-

cuitry may be affected by the ungrounded copper in this

solution. Unconnected copper conductors can collect a

capacitance which will dissipate uncontrollably.

In many instances, legends are used by equipment or indi-

viduals to evaluate the alignment of the BGA during the

placement operation. For peripheral leaded components,

the ﬁducial has been standardized so that placement equip-

ment can adjust the movement of the placement head

accordingly and improve the ﬁnal component positioning.

Local ﬁducials are often placed at opposite corners to allow

adjustment for the theta angle. This technique has been

incorporated into many placement tools and equipment.

The use of ﬁducials may not provide the most obvious

condition for human inspection; however, most inspectors

can approximate that the package is properly centered

between two ﬁducials in order to verify their position. In

some instances, companies have used angle brackets in

place of the ﬁducials to assist the human eye in making this

judgment; however, the camera for placement equipment is

not familiar with that conﬁguration, thus the practice is not

the most conducive for automatic assembly (see Figure

6-1).

Using silkscreen, the entire package can be outlined for

easy visual alignment. Another alignment pattern com-

monly used is to mark just the corners of the BGA pack-

age. Corner marks should only be 0.8 mm long on each

side. Copper can be used for corner marks, since it won’t

interfere with routing runs, as long as it does not affect cir-

cuitry performance such as unwanted capacitance.

All alignment legends should be offset 0.25 mm away from

the outer edge of the BGA package. This gives sufficient

clearance to view the features all around the BGA package.

Pin 1 identiﬁers are required on BGA land patterns. This

identiﬁer can be a caret, dot, or other easily visible shape.

The Pin 1 identiﬁer can be either silkscreen or copper and

IPC-7095c-6-1

Figure 6-1 BGA Alignment Marks

January 2013 IPC-7095C

Provided by IHS under license with IPC

Not for Resale

No reproduction or networking permitted without license from IHS

--`,,```,,,,````-`-`,,`,,`,`,,`---

should be distinct enough so as not to be confused with any

other markings around the land pattern.

6.2 Attachment Sites (Land Patterns and Vias)

6.2.1 Big vs. Small Land and Impact on Routing

The

diameter of the solder land can affect both the reliability of

the solder joints and also the routing of conductors. The

land diameter is usually smaller than the ball diameter of

the BGA. The land size reduction of 20 to 25% has been

determined to provide reliable attachment criteria. The

larger the lands the less room for routing between lands.

For example, a 1.27 mm pitch BGA package with 0.63 mm

diameter solder lands will be able to ﬁt two conductors

between the lands using 125/125 µm conductors and

spacing. If a 0.8 mm diameter solder land is used, only

one conductor can ﬁt between the solder lands using 125/

125 µm conductors and spaces.

Tables 6-1 and 6-2 show the number of conductors that can

be routed between lands for various land diameters and

conductor/space widths.

The following equation can be used to determine the num-

ber of conductors that can be routed between lands depend-

ing on package pitch (P), solder land diameter (D), number

of conductors between lands (n) and conductor/space width

(x).

P-D≥ (2n + 1)x

A general rule is to design the solder land on the circuit

board with the same diameter as the solder land on the

plastic BGA substrate.

Table 6-3 shows another view that takes the maximum land

size possible for a particular number of conductors instead

of number of conductors for each land size and has addi-

tional pitches. Information is also provided on interstitial

via.

Solder land sizes for a CBGA should be designed such that

the noncollapsing ball or column has sufficient platform

availability of the land in order to obtain the solder attach-

ment to the column or ball of the CBGA. This makes the

land somewhat larger in order to establish this minimum

requirement and is necessary to ensure reliability of solder

joints which usually comes from the melted solder paste

deposit.

6.2.2 Solder Mask vs. Metal Defined Land Design

There are two basic types of solder lands used for BGA

packages. These are metal deﬁned (MD) and solder mask

deﬁned (SMD). MD lands are etch-deﬁned and there is

solder mask clearance around the lands, similar to most

surface mount lands. SMD lands have solder mask overlap-

ping the copper land (see Figure 6-2). Both land types have

advantages and disadvantages.

6.2.2.1 Metal Defined Lands Metal-deﬁned (MD) lands

require a smaller diameter copper land and, therefore, have

more metal-to-metal spacing for routing and vias. Copper

dimensions can also be controlled better than solder mask

dimensions, giving a more uniform surface ﬁnish, espe-

cially for HASL boards. The absence of solder mask

around the solder land allows the solder to ﬂow around the

edges of the land, eliminating any areas of stress concen-

tration.

Metal deﬁned lands give the solder joint a much better

geometry but result in a lower standoff height (see Figure

6-3). This improved geometry may potentially improve

fatigue resistance; however, the lower standoff height may

negate some of the improvement to fatigue resistance.

6.2.2.2 Solder Mask Defined (SMD) Lands Because of

the overlapped solder mask, SMD lands require a larger

diameter metal land to achieve the same sized land diam-

eter as MD. The solder joint is deﬁned by the solder mask

creating a stress concentration (see Figure 6-4), but will

Table 6-1 Number of Conductors Between Solder Lands for 1.27 mm Pitch BGAs

Solder Land Diameter (micron) 750 700 625 500 400 350

Conductor

Spacing

Width (µm)

200N/AN/A1111

150111222

125112223

100222334

75233455

Table 6-2 Number of Conductors Between Solder Lands for 1.0 mm Pitch BGAs

Solder Land Diameter 625 500 400 350 300 250 200

Conductor

Spacing

Width (µm)

200N/AN/A11111

150N/A111122

1251112222

1001222233

752233444

IPC-7095C January 2013

Provided by IHS under license with IPC

Not for Resale

No reproduction or networking permitted without license from IHS

--`,,```,,,,````-`-`,,`,,`,`,,`---

have a higher standoff. The effect is illustrated in Figure

6-5, which shows the contrast in joint geometry resulting

from solder mask deﬁned lands (left side) and a metal

deﬁned condition (right side). The stress concentration on

the solder mask deﬁned land results in possible crack ini-

tiation at the mounting surface. The SMD lands adhere to

the board better because of the larger surface area of cop-

per and the overlapping solder mask. The major disadvan-

tage to SMD lands is the vulnerability of the solder joint at

the interface of solder mask and solder material. Some tests

indicate that the solder joint fatigue life has decreased sig-

niﬁcantly when compared with nonsolder mask deﬁned

(MD) lands. The major advantage is that this approach may

be used to prevent the land from pulling off of the board.

Land lifting, also known as cratering, usually occurs at the

corner balls. Because corner balls have a higher strain rate

and are more likely to fail, many times component manu-

facturers make these non-critical to function (CTF). In the

case of no CTF corner balls, it may be desirable to have

SMD lands in these locations.

6.2.3 Conductor Width The conductor width can affect

the routing of the BGA package. The wider the conductor,

the less room between lands for placing runs. There is no

Table 6-3 Maximum Solder Land to Pitch Relationship

Maximum Land Size

BGA Pitch Ball Size Standard Pad Via One Track Two Track

1.27 0.75 0.50 0.95 0.90 0.65

1.0 0.60 0.45 0.45 0.65 0.40

0.8 0.50 0.40 0.30 0.45 –

0.7 0.40 0.35 0.20 0.35 –

Assumption: 125/125 µm conductors and spaces

via land for 1.25 mm and 1.0 mm pitch BGA is 0.63 mm

via land for 0.8 mm and 0.7 mm pitch BGA is 0.5 mm

All values rounded down to 0.5 mm

IPC-7095c-6-2

Figure 6-2 Solder Lands for BGA Components

Copper Pad

Solder mask

away from pad

Via covered with solder mask for interconnection

Copper Pad

Solder mask

on pad

IPC-7095c-6-3

Figure 6-3 Metal Deﬁned Land Attachment Proﬁle

IPC-7095c-6-4

Figure 6-4 Solder Mask Stress Concentration

Solder Mask

Concentrates

Stress

Thermal Expansion

in “Z” Axis is Greater

for Solder Mask than

the Solder Ball

Cross Sectional

Area of Solder

Ball Reduced

January 2013 IPC-7095C

Provided by IHS under license with IPC

Not for Resale

No reproduction or networking permitted without license from IHS

--`,,```,,,,````-`-`,,`,,`,`,,`---