IPC-7095C-2013.pdf - 第67页

have a higher standof f. The ef fect 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 conc…

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

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

maximum conductor width recommendation for SMD sol-

der lands; however, the maximum conductor width con-

necting NSMD solder lands is 0.2 mm. Anything wider

will have the effect of changing the solder land to an SMD

type land at the location. For the same reasons, only one

conductor should be joined to any NSMD solder land. To

eliminate sharp corners, a ﬁllet should be used where the

conductor connects to the solder land.

6.2.4 Via Size and Location Vias can be placed between

BGA solder lands on the land pattern. Via lands should be

kept small enough to provide clearance between them and

adjoining solder lands. The maximum via size that can be

used depends upon the size and type (SMD vs. MD) of

solder land used. However, it is recommended that the

smallest standard via land/drill size be utilized for the

board thickness. Vias with 0.6 mm lands and 0.35 mm

drilled holes are common for 1.5 mm and 1.27 mm pitch

BGAs, while 0.5 mm lands/0.25 mm drilled holes are used

for 1.0 mm and 0.75 mm pitch packages.

To minimize the risk of solder bridging between standard

sized vias and solder lands, vias can be either tented or

have solder mask encroaching (overlapping) the via land.

Covering the via lands will also reduce the risk of narrow

solder mask dams peeling off during BGA rework. See

Figure 6-6 for examples of covered vias and narrow solder

mask dams. Tented vias may not be reliable with some

combinations of solder mask and surface ﬁnish. The solder

mask opening on an encroached via should be just large

enough to allow ﬂux and other contaminants to escape dur-

ing processing. Consult your board fabricator for capabili-

ties when planning to tent or use encroached solder mask

on vias. Also see Figure 6-7.

Other options for vias on BGA land patterns include blind

vias and microvias. Blind vias can be created using a stan-

dard drill process, laser ablation, or photo-deﬁned through

wet or dry (plasma) chemistry. The outer and inner layers

are sequentially built and are then laminated together.

Because the via penetrates only the outer layers, a smaller

sized drill can be utilized. However, this option is generally

a large cost addition. Blind vias can be placed between sol-

der lands but, because of their smaller via lands, centering

the via between the solder lands is not as critical.

Microvias are created in a secondary operation and pen-

etrate the outer layers only. A standard microvia connects

layers 1 and 2 and/or n-1 and n. A typical microvia can

have a 0.3 mm land with a 0.1 mm hole size. Because of

this small size, the via can actually be placed in the center

of the solder land with the only noticeable effect being a

small dimple. The dimple can be avoided by using a Type

VII via protection concept in the design that ﬁlls and caps

the via. By placing vias directly in the land, the space

between BGA solder lands on the outer layers can be used

exclusively for routing.

One should establish a liaison with a board manufacturer

for options and rules before designing BGA land patterns

with blind or microvias.

6.3 Escape and Conductor Routing Strategies Unlike

peripherally leaded packages, BGA solder joints are not all

easily accessible on the top board layer. This is especially

true for BGA packages with large, full grid arrays. Addi-

tional layers may be required to route the signals out from

underneath the middle of these packages.

For example, a 1.27 mm pitch, 357-pin PBGA has a 19x19

full grid array without the corner solder balls. If 0.63 mm

solder lands are used, this leaves only 0.63 mm between

lands for routing conductors. This would permit only one

0.2 mm conductor between the lands, meaning that only

the outer two rows (136 pins total) of the package could be

routed out on the top layer. All other pins (221 total) would

need to join to vias and then be routed out through other

signal layers. If 125 µm conductors/spacing is used, two

conductors could be placed between lands so that the outer

three rows of pins (192 pins total) could be routed out on

the top layer, leaving the remaining pins (165 total) to be

routed using vias.

The via pattern for the board requires much tighter feature

control as the pitch for BGA, FBGA and CSP becomes

smaller.

Fanout patterns should show a distinctive cross for power.

There have been instances that power isolation has

occurred when the cross pattern was not used in BGA

fanout due to power clearances, creating a wall around the

internal power pins. The cross pattern also allows for an

area for internal or cross BGA nets to route. (see Figure

6-8).

Successful BGA fanout involves:

• Adherence to a placement grid in alignment with the

fanout grid whenever possible

• Protecting BGA fanout vias during routing

• Proper via and land sizes

Figure 6-5 Solder Joint Geometry Contrast

SMD geometry

with stress-

concentration

MD geometry

without stress-

concentration

IPC-7095C January 2013

Provided by IHS under license with IPC

Not for Resale

No reproduction or networking permitted without license from IHS

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