IPC-SM-782A-表面贴装焊盘图形设计标准.pdf.pdf - 第29页

the design is memory , general logic, or analog, it is recom- mended that all component orientations are such that pin one orientation is the same. 3.6.1.4 Grid-Based Component Placement SMT com- ponent placement and ori…

3.6 Design Rules During the component selection phase

of a design, manufacturing engineering should be consulted

regarding any components outside the scope of this docu-

ment.

The printed board design principles are a statement of cur-

rent test and manufacturing capabilities. Exceeding or

changing these capabilities requires concurrence of all par-

ticipants in the process including manufacturing, engineer-

ing and test technology.

Involving test and manufacturing early in the design helps

to move a quality product quickly into production. Figure

3–7 shows a list of concurrent engineering team partici-

pants that should be involved.

3.6.1 Component Spacing

3.6.1.1 Component Considerations

The land pattern

design information discussed so far is important for reli-

ability of surface mount assemblies. However, the designer

should not lose sight of manufacturability, testability and

repairability of SMT assemblies. A minimum interpackage

spacing is required to satisfy all these manufacturing

requirements. There is no limit on maximum interpackage

spacing; the more the better. Some designs require that sur-

face mount components are positioned as tightly as pos-

sible. Based on experience, the examples shown in Figure

3–8 meet manufacturability requirements.

The land to land spacing between adjacent components

should be 1.25 mm [0.050 in] clear space all around the

edges of printed boards if boards are tested off the connec-

tor or 2.5 mm [0.100 in] minimum if vacuum seal for test-

ing is used. The requirements speciﬁed herein are recom-

mended minimums excluding conductor geometry

tolerances.

3.6.1.2 Wave Solder Component Orientation All polar-

ized surface mount components should be placed in the

same orientation, when possible. On any printed board

assembly where the secondary side is to be wave soldered,

the preferred orientation of devices on that side is

described and shown in Figure 3–9. The preferred orienta-

tion is used in order to optimize the resulting solder joint

quality as the assembly exits the solder wave.

• All passive components shall be parallel to each other.

• All SOICs shall be perpendicular to the long axis of

passive components.

• The longer axis of SOICs and of passive components

shall be perpendicular to each other.

• The long axis of passive components shall be perpen-

dicular to the direction of travel of the board along

the conveyer of the wave solder machine.

3.6.1.3 Component Placement Similar types of compo-

nents should be aligned on the board in the same orienta-

tion for ease of component placement, inspection, and sol-

dering. Also, similar component types should be grouped

together whenever possible, with the net list or connectiv-

ity and circuit performance requirements ultimately driving

the placements. See Figure 3-10. In memory boards, for

example, all of the memory chips are placed in a clearly

deﬁned matrix with pin one orientation the same direction

for all components. This is a good design practice to carry

out on logic designs where there are many similar compo-

nent types with different logic functions in each package.

On the other hand, analog designs often require a large

variety of component types making it understandably diffi-

cult to group similar components together. Regardless if

IPC-782-3-7

Figure 3–7 Simpliﬁed electronic development organization

▼

Admin-

istrative

control

Chain of

command

Operational

control

Working

level

PROGRAM

OFFICE

System

Manage-

ment

Project

Task

MANAGEMENT

ENGINEERING

MANAGEMENT

System

Engin-

eering

Elec-

tronic

Design

MANUFACTURING

MANAGEMENT

Product

Design

Fabri-

cation

Assem-

bly

Testing

Project

Task

Project

Task

Project

Task

Project

Task

Project

Task

Project

Task

Deliverable

Hardware

IPC-SM-782A December 1999

the design is memory, general logic, or analog, it is recom-

mended that all component orientations are such that pin

one orientation is the same.

3.6.1.4 Grid-Based Component Placement SMT com-

ponent placement and orientation is generally more difficult

than THT printed boards for two reasons: higher compo-

nent densities, and the ability to put components on both

sides of the board. For THT designs, the component leads

are on 2.54 mm [0.100 in] centers and, assuming 1.3 mm

[0.065 in] lands, the spacing between lands would be 1.2

mm. In high density SMT designs, however, the spacing

between lands is often less, down to 0.63 mm [0.025 in]

and smaller. Grid based component placement (0.100 inch

grid is standard with THT) is complicated by the large

variety of land sizes associated with the SMT component

packages now becoming available. Most SMT designs

being done today have abandoned the 2.54 mm [0.100 in]

IPC-782-3-8

Figure 3–8 Recommended minimum land-to-land clearances

Maximize View

Angle

for

Solder

Joint

Inspection

2.5 mm (0.100 in) Minimum

▼

1.25 mm (0.050 in)

1.5 mm (0. 060 in.)

0.63 mm (0.025 in.)

1.0 mm (0.040 in.)

1.0 mm

(0.040 in.)

▼

0.63 mm

(0.025 in.)

1.25 mm

(0.050 in)

1.5 mm (0.060 in.)

▼

DIP

IPC-782-3-9

Figure 3–9 Component orientation for wave solder applications

Wave Solder For SMT

Prefered IC orientation

Rubber pads will reduce

solder bridging

Typical solder

bridge locations

▼

Non Prefered IC orientation

December 1999 IPC-SM-782A

grid based placement rules of the THT boards. This ulti-

mately results in components being randomly placed, and

vias being even more randomly placed across the board.

Two problems created by random component placement

are a loss of uniform grid based test node accessibility and

a loss of logical, predictable routing channels on all layers

(possibly driving layer counts). In addition the accepted

international grid identiﬁed in IPC-1902 states that for new

designs the grid should be 0.5 mm, with a further subdivi-

sion being 0.05 mm. One solution to the problem is to

build CAD libraries with all component lands connected to

vias on 0.05 mm centers (or greater, based on design) to be

used for testing, routing, and rework ports. Then when

doing the component placement on the CAD system, sim-

ply place the components so that there is a minimum space

of 0.5 mm between lands, then snap the vias of the compo-

nent being placed out to the next 1.0 mm grid point. With

this procedure, all of the components should have between

0.4 mm and 0.6 mm (or an average of 0.5 mm) spacing

between the lands. From the assembly point of view, it is

easier to process a PCB which has the component centroids

on a 1.0 mm grid, with approximately equal spacing

between all of the lands across the board in both directions.

3.6.1.5 Single vs Double Sided Boards The term single

or double sided referred to one or two conductor layers on

a printed board prior to the advent of Surface Mount. Now,

however, the term single side refers to components

mounted on one side (Type 1 assembly), and the term

double refers to components mounted on both sides (Type

2 assembly) of the board. It has been observed that many

SMT designers, especially novices, are too quick to place

components on the secondary side of the PB, forcing the

assembly process to be executed twice instead of once.

Designers should concentrate on getting all components on

the primary side of the board whenever possible without

creating component spacing violations. This will result in a

lower assembly cost. If double sided placement is deﬁ-

nitely required, then grid-based placement, although more

difficult, is even more crucial for accurate ﬁnal component

placement, circuit routability, and testability. Double sided

boards using conventional SMT design rules often require

double sided, or clamshell test ﬁxtures that are 3 to 5 times

the cost of single sided test ﬁxtures. Grid based component

placements have been known to improve nodal accessibil-

ity as well as eliminate the need for dual sided testing.

3.6.1.6 Solder Stencil Design The solder stencil is the

primary vehicle by which solder paste is applied to the

SMT printed board. With it, the exact location and volume

of solder paste deposition is precisely controlled. The art-

work for the stencil generally consists of the component

mounting lands from the outer layers of the board with all

other circuitry deleted. The openings in the stencil should

be the same size as the lands on the board for all compo-

nents. The printed board assembler may alter the stencil

IPC-782-3-10

Figure 3–10 Alignment of similar components

Consistent

Orientation

PIN One I. D.

Uniform

Spacing

▼

PREFERRED LAYOUT FOR SMT

IPC-SM-782A December 1999