IPC-SM-782A-表面贴装焊盘图形设计标准.pdf.pdf - 第35页

need to use a soldermask to prevent the migration of solder away from the component land. B. Routing conductors into the lands as shown in Figures 3–20, 3–21 may restrict discrete component movement during reﬂow solderin…

shows a grid routing analysis with vias on 1.0 mm [0.050

in] centers. On the left side are listed the routing grids with

the actual routing channels denoted by solid triangular

points. It can be seen that with SMT geometry of vias

placed on 1.0 mm [0.040 in] centers, there is one routing

channel between lands using a 0.3 mm [0.012 in] grid with

0.15 mm [0.006 in] conductor width/clearances. The bot-

tom routing grid of 0.25 mm [0.010 in] with 0.125 mm

[0.005 in] has two routing channels between vias.

3.6.2.2 Surface Conductors Wide conductors connect-

ing to a land area can act as a solder thief by drawing sol-

der away from the land and down the conductor. Further-

more, if the conductor goes to a via which is connected to

an inner layer power or ground plane, the wide conductor

may act as a heat sink and draw heat away from the land/

lead area during reﬂow solder resulting in a cold solder

joint.

A. Narrow the conductor as it enters the land area. Maxi-

mum conductor width should be 0.25 mm [0.010 in]

(see Figure 3–19). The minimum conductor length

should be 0.50 mm [0.020 in]. This neckdown provides

an effective solder restriction, and may eliminate the

IPC-782-3-17

Figure 3–17 Surface mount conductor widths/clearances vs. routing grids

ROUTING GRIDS

.63mm

0.5mm

0.4mm

0.3mm

0.25mm

MANUFACTURING

ALLOWANCE

0.1mm

0.05mm

MINIMUM

CONDUCTORS/CLEARANCE

0.3/0.2mm

0.2/0.2mm

0.2/0.15mm

0.15/0.1mm

0.10/0.10mm

IPC-782-3-18

Figure 3–18 Section view of multilayer board with vias on 1.0 mm [0.040 in] centers

0.5mm SQ Land MIN 0.25mm DRILL

.5mm

GRID

.33mm

GRID

.25mm

GRID

.20mm

GRID

One

Track

Zero

Track

One

Track

Two

Track

.16mm .16mm

.18mm

.16mm .16mm

.125mm .125mm

.125mm .125mm.125mm

IPC-SM-782A December 1999

need to use a soldermask to prevent the migration of

solder away from the component land.

B. Routing conductors into the lands as shown in Figures

3–20, 3–21 may restrict discrete component movement

during reﬂow soldering. In the case of active IC’s this

routing geometry will allow the designer to use the

same library shape for surface routing or pad cap (no

surface routing) printed board conﬁguration. Addition-

ally, using this generic library shape allows ease of

switching between the two conﬁgurations midstream in

the design process without changing or editing compo-

nent libraries. In either case, 100% test node access is

retained. If wider conductors are required, the via land

size may be decreased accordingly to allow sufficient

spacing between the conductor and the land.

C. Use solder mask over bare copper (SMOBC) or copper

that has had the solder plating selectively removed.

The solder mask and bare copper provide an effective

barrier to solder migration. This may provide sufficient

protection even if options A and B are not possible.

3.6.2.3 Inner Layer Conductors The use of 0.2 mm

[0.008 in] conductors and clearance often drives layer

counts up because there is no routing channel available

between vias on 1.27 mm [0.050 in] centers. It is for this

reason that there is an increased usage of the conductors on

internal layers at or less than 0.15 mm [0.006 in] for SMT

designs, and 0.125 mm [0.005 in] conductors and clear-

ances for designs with heavy usage of FPT. Figure 3–22

and 3–23 show the number of routing channels available

between lands using the 0.15 and 0.125 mm [0.006 and

0.005 in] geometries. Since conductor width control is

much more difficult to maintain on outer layers of the PB,

it is better to keep the small geometries on the inner layers

of a multilayer printed board. Doing so may reduce the

need for soldermask and dramatically improve printed

board fabrication yields. Generally, the option of using

smaller geometries is driven by the need to reduce layer

counts. Decreasing layer counts may reduce the overall

board thickness and improve the aspect ratio for small hole

drilling.

3.6.3 Via Location Guidelines

3.6.3.1 Via Holes

Size of the via holes should be

selected based upon the printed board thickness vs. hole

diameter or aspect ratio limits as deﬁned by printed board

fabricator. In addition, speciﬁc via lands and holes can be

accessed for automatic in-circuit test (ICT). See 5.3.1. Fig-

ure 3–24 shows the land pattern-to-via relationships.

3.6.3.2 Vias and Land Pattern Separation Vias are

plated-through holes for example 0.63 mm to 1.0 mm

[0.025 to 0.040 in] diameter lands. They must be located

away from the component lands to prevent solder migra-

tion off the component land during reﬂow soldering. This

migration will cause insufficient solder ﬁllets on compo-

nents. (Solder drain) The solder migration can be restricted

by providing a narrow bridge between the land area and the

via or prevented by using the soldermask over bare copper

circuitry. (See Figures 3–19 and 3–20.)

The relationship for mounting land and via locations

should consider the conductor routing requirements. Figure

3–25 provides several examples of via positioning con-

cepts.

Specifying tented or ﬁlled vias will also reduce solder

migration on assemblies manufactured with a solder reﬂow

process. Filled or tented vias also take care of potential ﬂux

entrapment problems under components and are highly

desirable for attaining good vacuum seal during in-circuit

bed-of-nails testing. Tenting is done with a dry ﬁlm type of

soldermask, or the via may be ﬁlled with a resin prior to

liquid soldermask application.

3.6.3.3 Vias Under Components If the assembly is to be

wave soldered, via holes underneath zero clearance compo-

nents on the primary side should be avoided on boards

unless tented with soldermask. During wave soldering of

the assembly, ﬂux may potentially become trapped under

IPC-782-3-19

Figure 3–19 Narrowed conductor

IPC-782-3-20

Figure 3–20 Conductor routing

Conductors routing

away from lands

Conductors routing

to vias

December 1999 IPC-SM-782A

zero clearance devices. Via holes may be located under-

neath zero clearance surface mount packages in full surface

mount assemblies that will not be wave soldered. See Fig-

ure 3–26.

3.6.3.4 Vias as Test Points Via holes are used to con-

nect surface mounted component lands to conductor layers.

They may also be used as test targets for bed-of-nails type

probes and/or rework ports. Via holes may be tented if they

are not required for node testing or rework. When a via is

used as a test point it is required that the location of a test

land be deﬁned. See Section 5.0.

3.6.4 Standard Fabrication Allowances Manufacturing

tolerances or Standard Fabrication Allowances (SFA) exist

in all PB fabrication shops. Virtually every registration or

alignment operation that is performed has some potential

for misregistration. There are approximately 42 basic steps

in fabricating a multilayer PB, several of which involve

operations that require precision in location. They are as

follows: artwork generation, artwork tooling hole locations,

core material tooling hole size, inner layer image printing

operation, laminating ﬁxture tooling pin locations, material

shrinkage during lamination, drill tooling pin location, drill

x/y table tolerances, drill spindle tolerances, drill wander,

outer layer imaging, to name a few. The SFA considers all

of the tolerances of all the steps mentioned above. If all of

the equipment in a fabrication shop is old and worn the

SFA could be as high as 0.3 mm, whereas, a manufacturer

with new, precise equipment may have an SFA of 0.2 mm.

An industry average SFA of 0.4 mm may be used. The tol-

erance varies according to the printed board maximum

diagonal dimension and must be included in the land size

calculations. The fabricator should be consulted prior to

beginning a design to determine his SFA. With this num-

ber, the designer can proceed accordingly, preventing toler-

ances from stacking up and creating yield and/or produc-

tion problems. (See IPC-2221.)

3.6.4.1 Manufacturing Characteristics Figure 3–27

shows the various characteristics of conductor geometry.

End product drawings and speciﬁcations should specify

only minimums for conductor width and spacing. Tolerance

with plating of ±0.03 mm [±0.001 in] can be achieved

under special conditions. Artwork allowances that should

be incorporated into a design are shown in Table 3–8.

IPC-782-3-21

Figure 3-21 Surface routing geometries

SURFACE ROUTING GEOMETRIES

DETAILS OF THIS GEOMETRY:

Conductors and clearances may be 0.15 mm

Requires liquid photoimageable soldermask

100% Grid based test node accessibility from either side

0.8 mm

Square Via

0.6 X 2.0 mm

Component land

IPC-3-22

Figure 3–22 Conductor routing capability test pattern

2 Channel 2 Channel 3 Channel 3 Channel 4 Channel 5 Channel

IPC-SM-782A December 1999