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 > Embedded
> The Engineer’s Guide To High-Quality PCB Design

The Engineer’s Guide To High-Quality PCB Design

Jul 17, 2013
Nicholaus Smith
| Electronic Design

EMAIL

Tweet

Comments
14

Eventually, almost every EE must design a PCB, which isn’t something that’s
taught in school. Yet engineers, technicians, and even novice PCB designers can
create high-quality PCBs for any and every purpose with confidence that the
outcome will meet or exceed the objective.

Virtually every electronic product is constructed with one or more
printed-circuit boards (PCBs). The PCBs hold the ICs and other components and
implement the interconnections between them. PCBs are created in abundance for
portable electronics, computers, and entertainment equipment. They are also made
for test equipment, manufacturing, and spacecraft.

Sponsored

Fly-Buck
Converter PCB Layout Tips

High-Density PCB Layout of DC/DC
Converters

Eventually, almost every EE must design a PCB, which isn’t something that’s
taught in school. Yet engineers, technicians, and even novice PCB designers can
create high-quality PCBs for any and every purpose with confidence that the
outcome will meet or exceed the objective. Also, these designs can be completed
on schedule and within budget while meeting the design requirements. Designers
just need to mind the essential documentation, design steps and strategies, and
final checks.

Download
a special PDF version of this article, which is exclusive only to
Electronic Design community members.

The Basic Design
Process

The ideal PCB design starts with the discovery that a PCB is needed and
continues through the final production boards (Fig. 1). After
determining why the PCB is needed, the product’s final concept should be
decided. The concept includes the design’s features, the functions the PCB must
have and perform, interconnection with other circuits, placement, and the
approximate final dimensions.

Ambient temperature range and concerns regarding the operating environment
should be addressed and used to specify the materials selected for the PCB.
Components and PCB materials must be selected to guarantee operation under all
expected and potential forms of duress the board may be exposed to during its
lifetime.

The circuit schematic is drawn based on the concept. This detailed diagram
shows the electrical implementation of each function of the PCB. With the
schematic drawn, a realistic drawing of the final PCB dimensions should be
completed with areas designated for each of the circuit’s schematic blocks
(groups of components closely connected for electrical reasons or
constraints).

Bill Of Materials

Simultaneously with the schematic’s creation, the bill of materials (BOM)
should be generated. The components in the circuit should be selected by
analyzing the maximum operating voltages and current levels of each node of the
circuit while considering tolerance criteria. With electrically satisfactory
components chosen, each component should be reconsidered based on availability,
budget, and size.

The BOM must be kept up-to-date with the schematic at all times. The BOM
requires the quantity, reference designators, value (numeric value of ohms,
farads, etc.), manufacturer part number, and PCB footprint for each
component.

These five requirements are critical because they define how many of each
part are needed, explain identification and circuit locations while exactly
describing each circuit element used for purchasing and substitution, and
explain the size of each part for area estimations. Additional descriptions may
be added, but it should be a condensed list describing each circuit element, and
too much information can over-complicate library development and management.

Related

PCB
Designers Need to Know These Panelization Guidelines

Today’s
Intricate PCB Design Needs Evolved Tools

5
Proven Strategies for Reducing PCB Prototype Spins

PCB Documentation

The PCB’s documents should include the hardware dimensional drawings,
schematic, BOM, layout file, component placement file, assembly drawings and
instructions, and Gerber file set. User guides also are useful but aren’t
required. The Gerber file set is PCB jargon for the output files of the layout
that are used by PCB manufacturers to create the PCB. A complete set of Gerber
files includes output files generated from the board layout file:

Silkscreen top and bottom

Solder mask top and bottom

All metal layers

Paste mask top and bottom

Component map (X-Y coordinates)

Assembly drawing top and bottom

Drill file

Drill legend

FAB outline (dimensions, special features)

Netlist file

The special features included in the FAB outline include but are not limited
to notches, cutouts, bevels, back-filled vias-in-pad (used for BGA-type IC
packages that have an array of pins under the device), blind/buried vias,
surface finish and leveling, hole tolerances, layer count, and
more.1

Schematic Details

Schematics control the project, so accuracy and completeness are critical for
success. They include information that is necessary for the proper operation of
the circuit. A schematic should include adequate design details, such as pin
numbers, names, component values, and ratings (Fig. 2).

Embedded within each schematic symbol is the manufacturer part number used to
determine price and specifications. The package specification determines the
size of the footprint for each component. The first step should be to make sure
the exposed copper for each pin is in the proper location and is slightly larger
than the component pins (3 to 20 mils) depending on available area and soldering
method.

Consider assembly when designing footprints, and follow the manufacturer’s
recommended PCB footprint. Some components come in microscopic packages and do
not allow room for extra copper. Even in these cases, a stripe of 2.5 to 3 mils
of solder mask should be applied between every pin on the board.

Follow the rule of 10. Small vias have a finished hole size of 10 mils with
10 additional mils of pad ring. Traces should be 10 mils or further from the
edge of the board. Trace-to-trace pitch is 10 mils (5-mil air-gap, 5-mil trace
width, 1-oz copper). Vias with 40-mil diameter holes or larger should have a pad
ring added for reliability. An additional 15 to 25 mils of clearance beyond the
design rule should be instated for copper planes on outer layers from plane to
pins. This reduces the risk of solder bridging at all solder points.

Component Placement

Component placement is next in the process and determined based on thermal
management, function, and electrical noise considerations. A first-pass
component placement step commences after the outline of component and
interconnect position has been assigned. Immediately after the individual
components are placed, a placement review should be held and adjustments made to
facilitate routing and optimize performance.

Placement and package sizes are often reconsidered and changes are made at
this point based on size and cost. Components absorbing greater than 10 mW or
conducting more than 10 mA should be considered powerful enough for additional
thermal and electrical considerations. Sensitive signals should be shielded from
noise sources with planes and be kept impedance-controlled.

Power management components should utilize ground planes or power planes for
heat flow. Make high-current connections according to the acceptable voltage
drop for the connection. Layer transitions for high current paths should be made
with two to four vias at each layer transition.Place multiple vias at layer
transitions to increase reliability, reduce resistive and inductive losses, and
improve thermal conductivity.

Thermal Issues

The heat generated by the IC is transferred from the device to the copper
layers of the PCB (Fig. 3). The ideal thermal design will result in the
entire board being the same temperature. The copper thickness, number of layers,
continuity of thermal paths, and board area will have a direct impact on the
operating temperature of components.

To reduce operating temperatures easily, use more layers of solid ground or
power planes connected directly to heat sources with multiple vias. Establishing
effective heat and high-current routes will optimize heat transfer by means of
convection. The use of thermally conductive planes to spread the heat evenly
dramatically lowers the temperature by maximizing the area used for heat
transfer to the atmosphere (Fig. 4).2

With even heat distribution, the following formula can be used to estimate
surface temperatures:

P = (heatConvection) x area x
(ΔT)

where:

P = power dissipated on the board

Area = board (X axis x Y axis)

ΔT = surface temperature – ambient temperature

HeatConvection = convection constant based on ambient
conditions

Fine-Tuning The Component Placement

Components should be placed in the following order: connectors, power
circuits, sensitive and precision circuits, critical circuit components, and
then the rest. The schematic is built around each part on the PCB and completely
interconnected. Routing priority for the circuit is chosen based on power
levels, noise susceptibility, or generation and routing capability.

In general, trace widths of 10 to 20 mils are used for traces carrying 10 to
20 mA and 5 to 8 mils for traces carrying less current than 10 mA.
High-frequency (greater than 3 MHz) and rapidly changing signals should be
carefully considered when routed along with high-impedance nodes.

The lead engineer/designer should review the layout, and physical locations
and routing paths should be adjusted iteratively until the circuit is optimized
for all design constraints. The number of layers depends on power levels and
complexity. Add layers in pairs since the copper cladding is produced that way.
The routing of power signals and planes, the grounding scheme, and the board’s
ability to be used as intended all influence operation.

Final inspections should involve verification that sensitive nodes and
circuits are properly shielded from noise sources, solder mask exists between
pins and vias, and the silkscreen is clear and concise. When determining layer
stack-up, use the first inner layer below the component sides as ground and
assign power planes to other layers. Stack-ups are created in a manner that
balances the board relative to the midpoint of the Z axis.

Consider any concerns the PCB designer has during the reviews, and correct
the PCB based on feedback generated by the reviews. Create and verify lists of
changes during each review iteration until the board is finalized. During all
stages of the layout, keep the design error free by using the design rule
checker (DRC).

The DRC can only catch errors that it has been programmed to monitor, and DRC
rule sets often change based on individual designs. At the minimum, the design
rule checking should cover package-to-package spacing, unconnected nets (a
unique name identifying each node of the circuit), shorted nets, air-gap
violations, if vias are too close to solder pads, if vias are too close to each
other, and vertical clearance violations.

Many other important DRC rules can be set to ensure a robust design, and they
should be researched and understood. For example, keep clearances at or above 5
mils. Vias should not be located within surface-mount pads (unless back-filled).
And, solder mask should be between all solder points.

Cost is often a driving influence behind PCB design, so it is good to
understand the cost adders in PCB manufacturing. A typical board is two to four
layers, with no drill holes less than 10 mils in diameter and 5-mil minimum air
gaps and trace widths. It also should be 0.062 in. thick with standard FR-4 and
a copper foil weight of 1 oz. Additional layers, extra thick or thin boards,
vias-in-pad, back-filled vias (non-conductive preferred due to conductivity
limitations and thermal expansion differences), blind/buried vias, and lead time
all substantially add to the overall cost.

Manufacturer capabilities should be understood when the PCB design commences.
PCB fabs are routinely contacted about capabilities and cost reduction
techniques when designing PCBs for manufacturability.

Summary

PCB design may be complex, but it is quite possible to design good boards
with a little technique and practice. Using these guidelines and adding research
when needed, seasoned veterans may continue honing their skills and novice
designers may learn to create high-quality PCBs that exceed expectations.

References

1. Cohen, Patricio, Concepts and terminology used in Printed Circuit
Boards (PCB), Electrosoft Engineering, Web, May 25, 2013.

2. Mauney, Charles, Thermal Considerations for Surface Mount
Layouts, Texas Instruments, Web, May 13, 2013.

Nicholaus
Smith is an applications engineer at Integrated Device
Technology with more than 10 years of experience working on printed-circuit
boards (PCBs) and in semiconductor engineering. He was educated at the
University of Arizona and San Jose State University while working as a
technician and PCB designer. During his career, he has designed and used PCBs
for engineering evaluation, customer demonstration, IC qualification, and
automatic test equipment.

Sponsored

Fly-Buck
Converter PCB Layout Tips

High-Density PCB Layout of DC/DC
Converters

Print

reprints

Favorite

EMAIL

Tweet

Discuss this Article 14

CougFan

on Jul 24, 2013

I agree with your design flow except you left out one important input - the
mechanical design. How is the board going to be mounted? Are there keep outs?
Are there height restrictions? All these type of inputs are critical as well to
get the proper layout.

Log In or Register
to post comments

DHambley

on Feb 6, 2014

You might want to qualify your statement, "The ideal thermal design will
result in the entire board being the same temperature" for boards which only
have board-to-air cooling. In many applications though, the heat from hot parts
is directed to a heat sink which contacts the bottom of the board or to the
nearest mounting hole. In these cases the topology of Fig 3 should be altered so
that planes don't conduct heat to nearby IC's.

Log In or Register
to post comments

Smith
MP

on Oct 31, 2014

Nice to see this informative post about PCB and its design..
today, we
shared a post for newbies about How to design a Simple PCB step by step
tutorial....
Here is the link:

electricaltechnology.org/2014/10/pcb-designing-how-to-design-a-pcb.html

if the administration board of electronicdesign.com allow us, then we may
post it here for students and newbies in the blog section.
Thanks in
advance.

Log In or Register
to post comments

Advertisement

douglas11

on Nov 12, 2014

I have enjoyed learning from this ebook. I read the first 7 chapters in
detail and found them very helpful in designing my own custom PCBs (together
with data sheets/application notes from IC manufacturers, since this is not a
book about board layout or best practices in electronics). The examples are very
detailed and easy to follow. I continue to use this book as a reference for
various Eagle tools and tricks.

Douglas from http://hvactrainingpro.com/

Log In or Register
to post comments

user-463782

on Jan 29, 2015

garry-You might want to qualify your statement, "The ideal thermal design
will result in the entire board being the same temperature" for boards which
only have board-to-air cooling.
visit

Log In or Register
to post comments

user-463782

on Jan 29, 2015

You might want to qualify your statement, "The ideal thermal design will
result in the entire board being the same temperature" for boards which only
have board-to-air cooling.
visit

Log In or Register
to post comments

denisl

on Jun 5, 2015

There are many more issues to address such as controlled impedance traces,
differential pairs, high voltage clearances, ground plane and power plane,
minimum trace width and clearance, via aspect ratio, etc... If your board is
developed for being commercialized you better to rely on experienced PCB
designer and IPC certified. If you do not have these resources within your
company we can undertake the task, we offer this services.

Denis Lachapelle
http://www.sysacom.com/

Log In or Register
to post comments

PCB
Assembly

on Nov 4, 2015

Nice article. I have started my first electronic componet with one PCB design
for small project.
http://www.4pcbassembly.com/

Log In or Register
to post comments

Max
Black

on Nov 24, 2015

It's Nice and Helpful. After reading your article, I felt more clearly to
design PCB,there is one of my work,could you please give me some advices? Thanks
:)

easyeda.com/editor#id=ECYkF1ZlH3

Log In or Register
to post comments

user-959402

on Jan 31, 2016

I seriously love your blog.. Very nice colors & theme. Did you make this
site yourself? Please reply back as I’m looking to create my own site and would
love to find out where you got this from or just what the theme is called. Thank
you!
http://www.followersteam.com/

Log In or Register
to post comments

user-971502

on Feb 22, 2016

I seriously really like your weblog.. Very awesome shades & concept. Did
you make this website yourself? Please response back as I’m looking to make my
website and would really like to figure out where you got this from or just what
the concept is known as.

Log In or Register
to post comments

feeron

on Feb 28, 2016

You might need to qualify your announcement, "The perfect warm plan will
bring about the whole board being the same temperature" for sheets which just
have board-to-air cooling. In numerous applications however, the warmth from hot
parts is coordinated to a warmth sink which contacts the base of the board or to
the closest mounting gap .from www.pcdownloadfree.com/
we can download all our most loved applications free. i truly your aticle what
you said

Log In or Register
to post comments

Gastineau

on Mar 2, 2016

En même temps regarder les amis se réunissent et Nespresso (Bernays envoyer
câble) une copie de la Hublot Big Bang Ceci est une des nouvelles
passionnantes.

http://www.trustedmontres.com/

Log In or Register
to post comments

user-1015532

on Mar 9, 2016

great guide thanks for provide this ebook
www.bit.ly/1LE7XGa
www.bit.ly/1QR80KN
www.bit.ly/24FFTby

Log In or Register
to post comments

Please Log In or Register
to post comments.

Advertisement

Related Articles

PCB
Design And Its Impact On Device Reliability

New
Tools Help Tame PCB Design Work

What’s
New in Eagle V6 PCB Design Software? Prepare for More Third-Party Tools
1

Essential
Steps For Making High-Quality Electrical Measurements

Brighten
Up Your Bluetooth Designs With High-Quality Audio

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)
×