IPC-7351-2005_表面贴装焊盘布局设计和标准通用要求.pdf - 第31页

ｗｗｗ．ｂｚｆｘｗ．ｃｏｍ SMT printed board. W ith it, the exact location and volume of solder paste deposition is precisely controlled. The art- work for developing the stencil is the component mounting lands from the outer layers …

ｗｗｗ．ｂｚｆｘｗ．ｃｏｍ

See IPC-SM-785 and IPC-9701 for details regarding com-

ponent and assembly testing.

3.4 Design Rules The printed board design principles

recommended in this standard consider current test and

manufacturing capabilities. Exceeding the limitation of

these capabilities requires concurrence of all participants in

the process including manufacturing, engineering and test

technology. Involving test and manufacturing early in the

design helps to move a quality product quickly into pro-

duction.

Manufacturing engineering should be consulted regarding

any components outside the scope of this document.

3.4.1 Component Spacing

3.4.1.1 Component Considerations

The land pattern

design and component spacing affect the reliability, manu-

facturability, testability and repairability of surface mount

assemblies. A minimum inter-package spacing is required

to satisfy all these manufacturing requirements. Maximum

inter-package spacing is limited by several factors, such as

available board space, equipment, weight considerations,

and circuit operating speed requirements. Some designs

require that surface mount components be positioned as

close to one another as possible.

3.4.1.2 Wave Solder Component Orientation On any

printed board assembly where surface mount devices are to

be wave soldered, the orientation of devices in respect to

the solder wave can contribute to excessive solder process

defects. The preferred orientation compared in Figure 3-6

optimises the solder process, minimizing solder bridging

on the trailing or shadowed contacts as the assembly exits

the solder wave. All polarized surface mount components

should be placed in the same orientation when possible.

The following additional conditions apply:

a) All passive components should be parallel to each

other.

b) The longer axis of SOICs and the longer axis of passive

components shall be perpendicular to each other.

c) 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.

3.4.1.3 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. In memory boards, for example, all of the

memory chips are placed in a clearly deﬁned matrix with

pin one orientation in the same direction for all compo-

nents. This is a good design practice to carry out on logic

designs where there are many similar component types

with different logic functions in each package. On the other

hand, analogue designs often require a large variety of

component types making it understandably difficult to

group similar components together. Regardless of whether

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

mended (when possible) that the orientation of pin 1 on all

IC components is the same, provided that product perfor-

mance or function is not compromised.

3.4.1.4 Grid-Based Component Positioning SMT com-

ponent placement is generally more complex than PIH

printed boards for two reasons: higher component densi-

ties, and the ability to put components on both sides of the

board. In high-density SMT designs the spacing between

lands of different components are often less than 0.2 mm.

Grid-based SMT device placement may not be practical

due to the large variety of component shapes.

Two effects 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 (pos-

sibly driving layer counts). In addition, the accepted inter-

national 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 0.5 mm centers (or greater, based on design) to be

used for testing, routing, and rework ports.

It is easier to process a printed board (PB) that has uniform

component center-point spacing cross the board in both

directions (see Figure 3-7).

3.4.2 Single- and Double-Sided Board Assembly The

term single-sided board assembly refers to components

mounted on one side, and the term double-sided refers to

components mounted on both sides of the board. The

double-sided board assembly may require additional solder

and assembly process steps and can increase manufacturing

cost. Designers should concentrate on locating all compo-

nents on the primary side of the board whenever possible.

3.4.2.1 Solder Paste Stencil The solder stencil is the

primary vehicle by which solder paste is applied to the

IPC-7351 February 2005

标准分享网 www.bzfxw.com 免费下载

ｗｗｗ．ｂｚｆｘｗ．ｃｏｍ

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

of solder paste deposition is precisely controlled. The art-

work for developing the stencil is the component mounting

lands from the outer layers of the board with all other cir-

cuitry deleted. The information provided for the openings

in the stencil is usually indicated as being the same size as

the lands on the board for all components. This information

(or data) may be selectively modiﬁed by the printed board

assembler or process engineer who will deﬁne the speciﬁc

adjustments required to meet speciﬁc solder volume

requirements (see IPC 7525).

The optimum stencil thickness is determined by evaluating

the solder paste requirements for all the components to be

reﬂow soldered. This should be based on study of the mini-

mum and target requirements for SMT solder joints given

in IPC/EIA-J-STD-001.

Ideally, the volume deposited should be the total amount

required to achieve the ‘‘target’’ solder joint condition (see

IPC-A-610), less the solder already available on the land

and termination or lead (the latter can together amount to

10% to 20% of the total and should not be ignored). In

IPC-7351-3-06

Figure 3-6 Component Orientation for Wave-Solder Applications

Preferred Orientation

Defect Prone Orientation

Solder

bridging

Solder

Wave

Solder

Wave

IPC-7351-3-07

Figure 3-7 Alignment of Similar Components

Consistent

Orientation

Pin 1 I.D. Uniform

Spacing

February 2005 IPC-7351

ｗｗｗ．ｂｚｆｘｗ．ｃｏｍ

making calculations, it should be noted that the solder con-

tent of most pastes is 50% to 55% by volume (not by

weight), depending on particle size.

If the amount of solder paste to be deposited is less than

the amount provided by using an aperture at or near the

land area size, a reduced area of print should be placed in

the best position on the land to assure good wetting of the

joint areas. In some cases, this may best be achieved by

reducing the width of the print, in others, the length. For

very ﬁne pitch with inter-land gaps of less than 0.2 mm,

staggering (offsetting) the print at alternate ends of the

lands can reduce the risk of shorts after soldering.

If the amount of solder paste required is more than the

amount available using the geometry provided for the basic

land pattern on the PCB the aperture size in the stencil can

be enlarged to increase solder volume. The amount and

direction of the overhang of the printed solder beyond the

land is dictated by the space available around the land and

the need to avoid shorting and solder bridging if excess

overhang occurs. The tolerances on land position and print-

ing accuracy need to be considered when calculating the

maximum allowable over-print. See IPC-7525 for the

design and fabrication of stencils for surface mount solder

paste application.

3.4.3 Component Stand-off Height for Cleaning The

recommended minimum component stand-off height for

cleaning is affected by the distance across the diagonal of

the component lead pitch.

If a minimum stand-off cannot be achieved, proper clean-

ing under the component may not be possible. In this case,

it is recommended that a no-clean ﬂux be used and/or mask

material should be retained over all exposed via and circuit

patterns located under devices.

3.4.4 Fiducial Marks A ﬁducial mark is a printed art-

work feature created in the same process as the circuit art-

work for optical recognition systems. The ﬁducial and a

circuit pattern artwork must be etched in the same step.

The ﬁducial marks provide common datum points for all

steps in the assembly process. This allows each piece of

equipment used for assembly to accurately locate the cir-

cuit pattern. There are two types of ﬁducial marks.

3.4.4.1 Panel and Global Fiducials Global ﬁducial

marks are used to locate the position of all circuit features

on an individual board. When a multi-image circuit is pro-

cessed in panel form, the global ﬁducials are referred to as

panel ﬁducials (see Figure 3-8).

A minimum of two global ﬁducial marks is required for

correction of offsets (x and y position) and rotational off-

sets (theta position). These should be located diagonally

opposite and as far apart as possible on the circuit or panel.

A minimum of three ﬁducial marks is required for correc-

tion of nonlinear distortions (scaling, stretch and twist).

These should be located in a triangular position as far apart

as possible on the circuit or panel.

3.4.4.2 Local Fiducials Local ﬁducial marks are used to

locate the position of an individual component requiring

more precise placement.

A minimum of two local ﬁducial marks are required for

correction of translational offsets (x and y position) and

rotational offsets (theta position). This can be two marks

located diagonally opposed within or outside the perimeter

of the land pattern (see Figure 3-9).

It is good design practice to locate global or panel ﬁducials

in a three-point grid-based datum system as shown in Fig-

ure 3-10. The ﬁrst ﬁducial is located at the 0-0 location.

The second and third ﬁducials are located in the X and Y

directions from 0-0 in the positive quadrant. The global

ﬁducials should be located on the top and bottom layers of

all printed boards that contain surface mount as well as

through-hole components since even through-hole assem-

bly systems are beginning to utilize vision alignment sys-

tems.

All ﬁne pitch components should have two local ﬁducial

systems designed into the component land pattern to insure

that enough ﬁducials are available every time the compo-

nent is placed, removed and/or replaced on the board. All

ﬁducials should have a soldermask opening large enough to

keep the optical target absolutely free of soldermask. If

soldermask should get onto the optical target, some vision

alignment systems may be compromised due to insufficient

contrast at the target site.

If space is limited, one may be able to share a ﬁducial from

an adjacent component within the location constraint (see

Figure 3-10).

3.4.4.3 Size and Shape of Fiducial The optimum ﬁdu-

cial mark is a solid ﬁlled circle. The preferred diameter of

IPC-7351-3-08

Figure 3-8 Panel/Local Fiducials

Panel Fiducial

▼

Global Fiducial

▼

IPC-7351 February 2005

标准分享网 www.bzfxw.com 免费下载