Skip
to Navigation Skip
to Content

Electronic
Design

Search:

Store

Subscribe

About
Us

Contact Us

RSS

Advertising

Register
Log
In

Display
name or email address: *

Password:
*

Remember
me

Forgot Your
Password?

close

Technologies

4G

Analog

Android

Boards

Communications

Components

DSPs

Dev
Tools

Digital
ICs

Displays

Electromechanical

Embedded

FPGAs

Interconnects

IoT

Memory

Microcontrollers

Microprocessors

Passives

Power

Power
Sources

Test
& Measurement

WiFi

Windows

iOS

News

Products

Trends
& Analysis

Image Galleries

Markets

Automotive

Defense

Energy

Lighting

Medical

Mobile

Robotics

Learning Resources

Engineering
Essentials

Design
Solutions

What’s
The Difference Between…

Ideas
for Design

Salary
Survey

Salary
Calculator

White
Papers

Basics
of Design

eBooks

Webcasts

2015
Leaders in Electronics

Design
FAQs

Data
Sheets

Reference
Designs

11
Myths About...

Community

Ask
the Experts

Blogs

Bob
Pease

Contributing
Technical Experts

Engineering
Hall of Fame

Forums

Interviews

Our
Editors

STEM
Starter Tournament

Pop
Quizzes

Companies

Company
Directory

Part
Search

Advertisement

Home > Technologies > Boards
> PCB Designers Need to Know These Panelization Guidelines

PCB Designers Need to Know These Panelization
Guidelines

Dec 15, 2015
Jack Lucas
|
Electronic Design

EMAIL

Tweet

Comments
2

Unplanned delays and redesigns can be avoided by following common-sense PCB
processing edge and array guidelines, as well as understanding the basics of the
assembly methods.

Download
this article in .PDF format
This
file type includes high-resolution graphics and schematics when
applicable.

This
article provides common-sense printed-circuit-board (PCB) processing edge and
array guidelines that should give most assemblers a good chance at efficiently
populating the PCB assemblies (PCBAs) as designed. These guidelines are intended
for PCB designers, who must understand the basics of assembly methods (including
panelization concepts) applicable to their designs if there’s any hope they will
consistently turn out manufacturable board designs. These are also targeted at
the PCBA process technician trainee, so he or she will know what to ask for in a
PCB array design.

Guidelines spell out when to create arrays or add processing edges; the
proper sizes for arrays and processing edges; the type of breakout design that
should be used under given circumstances; and how to arrange breakouts to
prevent damage to individual PCBs when breaking them out of the array or while
removing processing edges.

Related

The
Engineer’s Guide To High-Quality PCB Design

Today’s
Intricate PCB Design Needs Evolved Tools

5
Proven Strategies for Reducing PCB Prototype Spins

This article uses the terms array and panelization interchangeably, whichever
seems to fit best at that time. It’s also common to use the term “matrix” for an
array of PCBs. It can get confusing, because the word “panel” is reserved for
the standard-size laminate piece used by the PCB fabricator, whereas the word
“panelization” indicates a method of designing an array of PCBs into a single
processing piece for the PCB assembler.

It’s impossible to come up with a set of hard rules for all due to the
differences in machine technologies from one assembly shop to another. In
addition, the PCB construction and thickness can play a major role in what rules
to use. To satisfy a variety of assembly shops and PCB construction
technologies, the PCB design has to be more robust—stronger panels, more
clearance of all types, more robust board finishes, etc. If you have a captive
assembly shop, you will have the flexibility to adjust some of the guidelines,
according to the assembler’s unique capabilities, when product design density
dictates the need.

PCB Processing Edge or PCB Array

Small boards

Most production machinery, paste printers, pick-and-place machines, AOI
equipment, selective soldering machines, wave-solder machines, transfer
conveyors, etc., cannot process boards with less than a 2.0-in. (50.8mm)
conveyor width. So when the longest side of a rectangular PCB is less than 2.0
in., you must either add processing edges to make it bigger or create an array
of boards, or a combination of the two.

Odd-form boards

When a PCB needs to fit into an odd-form space and doesn’t have two parallel
edges for processing on conveyors, one must somehow add the necessary processing
edges. These make for some pretty interesting and complex array designs, keeping
in mind how the boards will be depanelized and how board cost is minimized by
making them fit well on the fabricator’s standard processing panel. These
considerations are covered below.

Note: You do have the option of using an adjustable or custom-made
board carrier, but these options are pretty expensive and cumbersome. They can
also be maintenance-intensive and use up significant floor space.

Board-Array Dimensions

You should design your PCB array to secure the benefits of running multiple
boards through your processes, while yielding the maximum number of boards from
the PCB fabricator’s standard processing panel. Every cut in the array that’s
made to facilitate future PCB breakout will weaken the panel somewhat.
Therefore, you must also limit the size of the array to prevent PCB-array
weakness, which can cause vibration in the pick-and-place machine and sagging in
the wave-solder machine.

The typical PCB manufacturer runs a standard panel size of his choice, very
commonly 18 × 24 in. They will want a 1/2-in. perimeter clearance for handling
the panels when processing double-sided boards and a 1-in. clearance when
processing multilayer PCBs. On an 18- × 24-in. panel, this translates to 17 × 23
in. of usable panel space for double-sided and 16- × 22-in. inch panel space for
multilayer boards. They will need about 0.1 in. of routing space between board
arrays, so this is also unusable panel space. A number of “panel calculators”
are available for use to help maximize the board count you get from the
fabricator’s standard panel; however, if you don’t get 70% usage, you should try
harder (Fig. 1).

The other item to consider when designing the panel size is to keep the
conveyor width changes to a minimum. This is especially important in the
low-quantity, high-mix world in which I live. If you’re running millions of
identical boards down a line, then this isn’t a big concern.

In one example of limiting the conveyor width changes, the following array
widths were developed to use the 24-in. dimension of the fabricator’s panel
efficiently with a 1-in. perimeter handling clearance:

W = 3.75 in., L ≥ W

W = 7.25 in., L ≥ W

W = 10.75 in., L ≥ W

The length of the array is then subject to the 16-in. limitation of the
18-in. panel edge.

Panelization Methods

The design of the board—namely how much component clearance is provided on
the edges, whether sensitive SMT components are close to an edge, and whether or
not connectors or other components hang over an edge—will limit the choices of
panelization breakout methods from which to choose. Sometimes a combination of
methods is appropriate to secure the PCB-array strength, while providing a
viable breakout method.

To improve strength, increase the board count on the fabricator’s panel, and
facilitate automated depaneling, arrays can be designed with solid tabs between
boards in just about any orientation. The depaneling method for this kind of
panel is either a depaneling router or a laser-cutting machine. The former
creates vast amounts of dust, noise, and vibration, and requires firm holding
fixtures. The latter is capital-intensive and limited to board thicknesses of
about 1 mm. Still, these methods have their place in the high-volume market and
aren’t subject to many of the restrictive guidelines to be outlined later.

The solid tabs between boards can be removed with a hook-shaped blade tool,
but this process can be troublesome. Even with very little clearance of the
blade in the slot between boards, it can rotate and take a bite out of the good
part of the board. If the blade-cutting edge is tapered to prevent board damage,
it leaves a little of the tab protruding from the good board. It’s also a very
inefficient process.

The two preferred depanelization methods for the low-volume/high-mix arena
are V-grooves and perforated tabs. Tabs and V-grooves are pretty well covered in
the IPC standards.

V-Groove Panelization Method

Generally speaking, this calls for cutting 1/3 the thickness of the board
from the top and 1/3 the thickness from the bottom, collinear with the top cut,
with a 30- to 45-degree circular cutting blade. A machine is needed to depanel
it, as the remaining 1/3 of the board thickness left intact is surprisingly
strong, and breaking it off by hand would put severe stress on the PCB.

Many prefer the V-groove method (Fig. 2) where possible (in which no
components hang over the edge), because it’s more efficient and produces less
surface stress when using a properly designed machine known as a “pizza cutter.”
Also, the pizza-cutter-type depaneling machines for V-grooves are inexpensive,
last forever, and require very little adjustment and maintenance. Furthermore,
they’re portable—you can mount the depaneling machines on a small cart and
easily move them around the shop wherever they’re needed.

However, this is the most restrictive method of panelization. For example,
you can’t use a V-groove breakout method where components are hanging over the
edge. Even if they’re too close to the edge of the board, you can’t use this
method unless you’re cutting a straight line all the way through the PCB
array.

To clear the circular cutting blade, you must maintain 0.05-in. clearance
from components to the center of the V-groove score, taking into consideration
component size and mounting variations. Tall components, such as radial
capacitors, radial inductors, and power-dissipating radial ceramic resistors,
would have to be spaced greater than 0.05 in. (nominal) because of position
variation, whereas connectors and other low-profile parts may be placed at
0.05-in. clearance.

Surface-mount multilayer ceramic chip capacitors (MLCCs) must be oriented
with the long side parallel to the V-groove cut if less than 0.25 in. (6.35 mm)
away from the score line and kept 0.119 in. (3 mm) away regardless. This becomes
more important with the larger-size caps and with certain cap dielectrics. The
surface stress, caused by forcing the depaneling blade into the V-groove,
transfers through the board surface to the rigid solder joints, and then to the
component bodies. This can fracture them if they're too close to the V-groove.
Orienting the long edge of the capacitor body parallel to the edge minimizes the
risk of body fracture (Fig. 2, again).

V-grooves can also weaken a PCB array, which is very undesirable when the
array must go through a wave-solder machine. The surface tension of the solder
wave, pulling down on the preheated PCB material, is exacerbated by V-grooves in
the array. When the board is pulled down, the protruding leads tend to run into,
and sometimes get hung up, on the wave-solder baffle.

In the case of a rectangular PCB, you would strengthen the array by “jump
scoring” on the shorter, or leading and trailing, edges (Fig. 3). Since
the V-groove blade is circular, you must cut beyond the edge of the board to
achieve a full-depth V-groove at the edge of the board. Running the cut 1/4 in.
past the edge of the PCB, halfway through a 1/2-in. breakaway edge, will leave
enough of the leading and trailing edges to strengthen the array and minimize
the pulling down effect of the wave, while achieving the desired full depth
V-groove cut on the board.

When jump scoring is used, the depaneling operators must be instructed to
remove the leading and trailing edges before trying to separate the boards. You
may get some push back from the PCB fabricator, but it gives you a stronger
array. Give the fabricator a break by not dimensioning the end of the jump
score. It’s hard to control, and you don’t know the V-groove cutting-blade
diameter. So you don’t know exactly where the cut will end.

Note: The V-groove method is undesirable if a “clean,” smooth board
edge is required, but this is rarely the case.

Breakaway-Tab Panelization Method

When V-grooves can’t be used, design PCB arrays, leaving perforated tabs
routing space between PCBs. Keep traces and surface-mounted parts 1/8 in. or
about 3 mm away from the perforation holes in the tabs to avoid damage from
splintering and surface stress during board separation. Keep the SMT MLCCs 1/4
in. (6.35 mm) away from the perforated-tab holes. Standard router size is 3/32
in. or 2.5 mm in most fabrication houses, and you want to design a spacing that
requires a single pass of the router bit. Where array weakness was a
consideration for V-groove designs, it’s doubly so for perforated-tab
arrays.

A five-hole perforation pattern is standard for breakaway tabs. Three-hole
patterns, which are for knockouts, may be used where trace or component edge
clearance is limited and where tabs must be placed under overhanging parts. The
three-hole breakouts, being much weaker, must be spaced closer together than the
five-hole breakouts.

Removable knock-outs are required to fill holes with area greater than or
equal to 0.6 in.2, to prevent the solder wave from running onto the
top of the board. In the case of a relatively small, rectangular knockout, a
single five-hole breakout tab may be placed on any one side. Since PC boards
will sag in the middle over the wave, knockouts are more important toward the
middle of the board and less important toward the edges. If the wave-solder
process isn’t necessary, the knockouts aren’t required.

The breakout-tab specifications, adapted from IPC-7351 (Fig. 4), are
designed to prevent the leftover material from the tab perforations from
protruding past the PCB edge after breakout. This may cause some headaches for
the PCB designer when running traces near the board edge, but it can usually be
accomplished if kept in mind from the beginning of the board design.

Perforated holes, centered in the routed cutout, will cause unwanted side
board protrusions (Fig. 5).

Three-hole perforated tabs are used for knockouts and for board edges when
there’s not enough room for five-hole perforated tabs. A rectangular knockout
can be designed with a five-hole perforated tab on any single edge (Fig.
6).

Do not place breakaway tabs under overhanging components (Fig.
7).

Tabs must be placed as close to the ends of the panel as possible to prevent
"whale finning" (Fig. 8) and thereafter, every 2 to 3 in. for five-hole
pattern or 1.5 in. for three-hole perforated tabs. Three-hole pattern breakouts
are used on board edges where space and clearance prevents use of five-hole
breakouts.

Three-hole pattern breakouts are used on board edges where space and
clearance prevents use of five-hole breakouts.

The breakaway panels must be designed so that all tabs broken at one time are
collinear. Another way to state it is that the break axis must be collinear with
the tab hole perforations involved in any one break. If the tab perforations
aren’t collinear during the breaking operation, some tabs will experience a
force perpendicular to the board surface, causing a tearing action on the
surface lamination (Fig. 9).

It could be just the solder-mask layer that delaminates and gets separated
from the traces, or it could actually be the surface layer of the board that
tears and pulls up any traces with it. This is a main complaint against the
perforated-tab method of panelization. At AMETEK, we have found a breaking method that will never
damage a board, which is described below. In practice, though, this method IS
NOT foolproof.

Combining Panelization Methods

Putting the guidelines together for the V-groove and perforated-tab
panelization methods, let’s look at two array designs for the same board
(Fig. 10).

The good design reduced the board count on the fabricator’s panel. However,
it was well worth paying slightly more for the PCBs in order to prevent the
board damage that kept occurring during breakout and the problems with the
wave-solder overflow.

Critical Instructions for Breaking Out Boards with Perforated
Tabs

No matter how well you design a perforated-tab PCB array, the possibility
exists for tearing or splintering the solder-mask layer, or the active surface
layer, of the PCB if a poor method of break out is used. The following is a safe
method of breaking out perforated-tab arrays, to both minimize PCB damage and
the stresses transferred across the PCB’s surface to the components during
breakout (Figs. 11 and 12).

Panel-Strength Considerations for Multiple Board Arrays

The main reasons for maintaining overall panel strength is to avoid vibration
in the pick-and-place machine and droop during wave soldering and selective
soldering. The rules outlined below may be relaxed by 50% if the panel will not
be subjected to any form of through-hole machine soldering. They also may be
relaxed if the panel will be soldered on a supporting pallet. Following are some
guidelines to assure sufficient panel strength to withstand processing
stresses.

V-groove scoring or breakout tabs with routing between boards cause
significant reduction in panel strength. The number of V-grooves or routings
between boards on a multiple image pallet must be limited, depending on:

• Board material and thickness

• Weight of parts to be installed on the board

• Whether or not the boards will be processed through soldering machines,
using a rigid soldering pallet

Multiple board panels must be designed in a way to provide leading and
trailing unscored stiffener edges. Use jump scoring, as described earlier in the
article, as necessary. If heavy parts must be hand-soldered because they can’t
withstand automated soldering processes or because they’re on the bottom side of
the board, they’re not a factor in panel design decisions.

For FR4 or HTFR4 PCBs greater than or equal to 0.06 in. (1.5 mm) thick, allow
no more than five boards, side by side, up to 1.5-in. board width, four boards
up to 2.5-in. board width, three boards up to 4-in. board width, and two for
boards up to 7.5-in. board width.  Boards up to 6.65 in. long may be turned
90° on the panel and placed side by side along the long axis of the array to fit
within the standard 7.25-in. width. This only makes sense if the resulting panel
is longer than it is wide, so you can add boards to the array to utilize the
fabricator’s panel efficiently (Fig. 13).

You may also attempt to rotate longer boards, up to 10 in. long, 90° to fully
utilize the fabricator’s panel. However, that usually results in excessive array
droop during through-hole machine soldering. Rotating the longer boards is more
practical on thicker, more robust PCBs. When designing the standard,
0.09-in.-thick PCBs, the board count can increase in the arrays above these
guidelines.

For FR4 or HTFR4 PCBs less than 0.06 in. (1.5 mm) thick, allow no more than
three boards side by side, up to 1.5-in. board width, and two boards, up to
3-in. board width. Note that these panels will be extremely fragile and still
not be wave-solderable without being supported by a wave pallet.

Another consideration during PCB-array design, to avoid drooping in
processing machines, is the weight of the parts on the board. If the boards will
have heavy magnetics (greater than a half a pound or 1.1 kg) or other massive
parts on them, it’s best not to put multiple boards on a panel. Two boards with
heavy parts may be placed side by side if the resulting panel width is no more
than 7.25 in. In this case, it’s best to specify a thicker PCB, say 0.09 in.

Miscellaneous Considerations

Odd-shaped PCBs: Odd-shaped boards may be rotated with respect to
each other to reduce PCB raw material waste, thus reducing board cost. It’s
acceptable to alternate the images, 90° to 180° from each other, to realize the
savings in PCB material, as long as you don’t violate the rule about breakout
tab perforations being collinear with each breakout axis.

Tooling holes: To facilitate bed-of-nails testing, provide tooling
holes near any three corners of the board arrays on the breakaway processing
edges. Tooling holes are typically 0.125 in., +0.004/-0.00, and are unplated.
Also, tooling holes are usually placed about 5 mm from the edge of the
board-array edges.

Fiducial marks: Arrays that contain PCBs with surface-mounted parts
must have fiducial marks, typically one near each tooling hole. There are many
choices for fiducial-mark formats, so you should consult your assembler for
their preference. The edges of the fiducial marks must be at least 0.157 in. (4
mm) from the board edges so that they don’t get obscured by conveyor top clamps
in the processing machines with fiducial-alignment camera systems. The array
processing-edge fiducial marks don’t preclude the necessity of providing
fiducial marks on the individual boards within the array.

Conclusion

No designer can afford to ignore such PCB panelization considerations.
PCB-array designs may dramatically impact, either positively or negatively, the
PCB assembly process. The various considerations are complex and will be
affected by PCB geometry, as well as the myriad of machine capabilities of
countless PCB assembly service suppliers. PCB cost can also be significantly
affected by the array design.

The above guidelines aren’t set in cement, but they work for us as good
practice in AMETEK production applications. You should always try to connect
with your PCB assembly service to become familiar with its capabilities and
machine process requirements. But since this is often impossible during the
design phase of PCBs, try to design on the robust side to improve your chances
of achieving an efficient assembly process.

Print

reprints

Favorite

EMAIL

Tweet

Discuss this Article 2

jimfordbroadcom

on Dec 17, 2015

Excellent article! As a PCB design engineer, it was an eye-opener to me as
to the reasons behind some of the requirements we get from our captive assembly
shop. Part of our PCB design process is that as soon as parts placement is
finished, we e-mail the top and bottom assembly layers of a board to the
assembly shop, and they respond in a day or so with panelization
recommendations. These include dimensions and locations of fiducials, tooling
holes, V-grooves, routed channels, mouse-bites, and board replica locations and
orientations. We incorporate their recommendations into our fab drawing as a
separate layer. Thanks!

Log In or Register
to post comments

waledkhan99

on Mar 2, 2016

Nice Job Done

regards,
http://www.mobdroforpc.org/

Log In or Register
to post comments

Please Log In or Register
to post comments.

Advertisement

Related Articles

The
Engineer’s Guide To High-Quality PCB Design 14

Today’s
Intricate PCB Design Needs Evolved Tools 2

5
Proven Strategies for Reducing PCB Prototype Spins

Digital
Modeling Yields Efficient Rigid-Flex PCB Design Processes

A
Quick Tutorial on PCBs

Search Parts

G0

powered by:

Advertisement

ED Top Articles

Gallery:
The Future of Transportation

Comparing
Ada and C

Electronic
Design’s Products of the Week (1/24-1/30)

CES
2016 Roundup, Part I

Play
Ball with IoT Indoor Positioning Sensors

Advertisement

Commentaries and Blogs

A
Tale of Two Bluetooth Headsets

Posted 3 years ago

in The
Testbench

Episode
26: TI App; AUVSI Highlights

Posted 4 years ago

in Engineering
Radio

Binary-Blended
Polylactic Acid Multilayer Film Exhibits Super Piezoelectric Effect

Posted 3 years ago

in Component
Connection

Thinking
About Communications, and a Farewell

by Don
Tuite

Posted 50 weeks ago

in Secondary
Emissions

Five
companies to look out for at Embedded World 2014

by Sally
Ward-Foxton

Posted 2 years ago

in Crosstalk

Have
Smartphones Peaked?

by Lou
Frenzel

Posted 1 week ago

in Communiqué

Passive
Components Still See Ink And Innovation

by Joe
Desposito

Posted 2 years ago

in Joe
Desposito's Blog

Are
micro:bits the Right Way to Teach STEM?

by William
Wong

Posted 5 days ago

in alt.embedded

Malicious
Malware Could Grab Your Christmas Cash

by Paul
Whytock

Posted 1 year ago

in London
Calling

Home
or Very Small Office Electronic Circuit Prototypes, Part 4

by Roger
Watkins

Posted 4 weeks ago

in Guest blogs

1-GHz
IsoVu Leads Tektronix Probe Performance/Usability Charge at APEC

by Patrick
Mannion

Posted 1 week ago

in Test.Pass

Expectations
for APEC 2016

by Maria
Guerra

Posted 6 weeks ago

in Charged Up

Advertisement

Contributing Technical Experts

JESD204B
Simplified

by Richard
F. Zarr

Published on Oct. 15, 2015
in ADC

Moving
to Deterministic ICE

by Lauro
Rizzatti

Published on Feb. 25, 2016
in Test
& Measurement

User-Programmable
FPGAs: The New Frontier of Instrumentation

by David
Hall

Published on Nov. 18, 2015
in Test
& Measurement

Understanding
and Measuring Power-Supply Transient Recovery Time

by Bob
Zollo

Published on Feb. 18, 2016
in Test
& Measurement

Does
Inductor Ripple-Current Percentage Still Matter in Low-Power Step-Down
Converters?

by Chris
Glaser

Published on Nov. 23, 2015
in Power

Guest Blogs

Mar 2, 2016

Article

Home
or Very Small Office Electronic Circuit Prototypes, Part 4 1

Part 4 focuses on testing for a reflow oven and
build of a mixed SMT/through-hole board....More

Jan 4, 2016

blog

Building
Home or Very Small Office Electronic Circuit Prototypes, Part 3
7

Part 3 delves into critical equipment for testing
today's electronics, and provides updates on circuit-board designs from Part
1....More

Nov 16, 2015

Commentary

Building
Home or Very Small Office Electronic-Circuit Prototypes, Part 2
7

Part 2 gives step-by-step instructions on how to
turn a Black & Decker TO1675B convection countertop oven into a
temperature-controlled reflow oven....More

Search Parts

Powered
by:

The Original Electronics Parts Search And Procurment Tool

Connect With Us

Twitter

Facebook

RSS

Advertisement

ElectronicDesign.com

Technologies

News

Markets

Learning
Resources

Community

Companies

Part
Search

Site Features

Media Center

Newsletters

RSS

Site Archive

Sitemap

Submit
Articles

View
Mobile Site

Penton Corporate

About Us

Privacy Policy

Terms of Service

Contact
Us

Follow Us

Twitter

Facebook

RSS

Search ElectronicDesign.com

Search:

PISCES

Electronic Design Related Sites

Machine
Design

SourceESB

Microwaves &
RF

Power
Electronics

Hydraulics & Pneumatics

Medical
Design

Engineering
TV

Defense
Electronics

Global
Purchasing

Electronic
Design Europe

Advertisement

Advertisement

Advertisement

Copyright © 2016 Penton

Sponsored Introduction Continue on to
(or wait seconds)
×