Practical Electronics/PCB
Layout

From Wikibooks, open books for an open world

< Practical
Electronics

Jump to: navigation,
search

The efficient laying out of traces on a PCB is a complex skill, and requires
much patience. This task has been made vastly easier with the advent of readily
available PCB layout software, but it is still challenging.

Usually an electronics or electrical engineer designs the circuit, and a
layout specialist designs the PCB. PCB design is a specialized skill. There are
numerous techniques and standards used to design a PCB that is easy to
manufacture and yet small and inexpensive.

These are the usual steps in PCB layout for most customers that allow the
customer maximum flexibility to make changes to embrace the normal engineering
changes that happen during the design process. By utilizing this structured
approach maximizes the engineering teams' efforts to design and build a
successful product.

1. Schematic / Components design review. 2. Determine what footprints are
required to be built, and build them incorporating 3D models. 3. Board outline
definition process. DXF board outline file import is the most stable method. 4.
Component placement. 5. Customer review of component placement. 6. Power and
Ground Plane assignment. 7. Customer review of Power Plane and Ground Plane
Assignments. 8. Fanout. 9. Critical net routing. 10.Customer review of critical
net routing. 11. Non critical net routing. 12. Customer review. 13. Silkscreen
adjustment and board part number assignment/placement. 14. Gerber, DXF, Step,
IDF/LDF final file generation for final customer review and approval. 15. Final
cleanup and any touch up required from customer feedback.

[1]

Contents

1 Copper
Thickness

2 Trace Width

3 Footprints or
Geometries

4 Holes

5 Board Thickness and
Layers

6 Trace
clearance

7 Remove less
copper

8 Fiducial

9 Via

10 Solder mask and
silkscreen

11 Basic
guidelines

12 Further
Reading

13 References

14 External
links

Copper Thickness[edit]

The vast majority of PCBs are manufactured with "1 ounce copper" on the outer
layers. If there are inner layers, they are almost always manufactured with "1/2
ounce copper".

The thickness of the copper layer on the PCB affects the behaviour of the
circuit. PCB copper thickness is usually measured in ounces per square
foot, or frequently, just ounces. It can also be given in micrometres,
inches or mils. The measurements for commonly used thickness are given
below.

oz/ft²

μm

in

mil

0.5

17.5

0.0007

0.7

0.75

25.5

0.0010

1.0

1

35

0.0014

1.4

2

71[2]

0.0028

2.8

3

105

0.0042

4.2

As always, the thickness of a thin slab of metal with a given top surface
area is always exactly

The area is "1 square foot" (144 square inches), the density of copper is
8.96 mg/mm3 = 5.18 ounce/(inch3), and usually the mass is
"1 ounce of copper", but occasionally 1/2, 2, 3, or 4 oz.

Trace Width[edit]

Different widths of traces have different properties that could affect the
operation of the circuit. For, example, a thin trace has a higher resistance
than a thick one, and can therefore carry less current or will heat up more for
the same current.

Due to the large number of tables and charts, this information is presented
on different pages:

For current capacities, see Trace
Current Capacity.

Most manufacturers can manufacture a minimum trace width of 0.006 inch. (Many
can manufacture traces 0.004 inch wide). Such minimum-size traces are more than
adequate for most digital and analogue signals.

Footprints or
Geometries[edit]

The manufacturer of each part recommends a "footprint", a copper pattern for
the part to be soldered to the PCB.

Sometimes the footprint also includes a drawing of the outline of the part.
Some people put that outline on the silk screen. Other people make a "virtual
outline" that shows up on the computer screen and on the assembly drawings, but
not on the actual PCB.

Footprints for capacitors and batteries should include plus sign (+) polarity
marking on the silk screen next to the positive pad. (The positive-end-indicator
stripe on the capacitor itself should be placed nearest that plus sign).

Footprints for LEDs and other diodes should have a polarity mark -- the
"diode arrow symbol" (triangle + bar), or at least the bar, in silk-screen. The
bar matches the cathode-end-indicator stripe on the diode itself. [3]

Footprints for ICs should have a polarity mark "dot" or "1" near pin 1. Most
people give pin 1 a "squared-off" pad, and all other pins a "rounded pad". Some
people also like additional "10", "20", "30", etc., marks in silkscreen next to
pin 10, pin 20, pin 30, etc.

The polarity mark must be visible after mounting the part so it can be seen
after inspection. (It's useless to put the polarity mark where no one can see
it). It's okay to put the polarity mark underneath a tubular-packaged diode,
since people can look "around" the mounted diode and see the polarity mark. [4]

Holes[edit]

There are 3 general types of holes:

A via -- literally, a "way" to get from one layer of copper to another
layer of copper. The vias on a particular PCB should all be the same size. Some
people[10] recommend 0.025" (0.6mm) diameter via holes, surrounded
by a 0.0394" (1.0mm) diameter via copper pad, if at all possible. Some very
dense SMT boards require smaller vias. Some manufacturers can handle 0.012"
diameter via holes, surrounded by 0.024" diameter via pad.

Since there is no actual component put into a via, many PCBs are manufactured
with "plugged" vias (vias completely filled with metal) and "tented" vias (vias
completely covered with solder mask).

A through-hole -- many components (called "through-hole components")
require a hole (a "through hole") for each pin. The part manufacturer should
specify a "footprint" including the location and size of each hole. If there is
no recommendation, common practice is

round leads: add 6 mils to the nominal round lead diameter to get the
recommended PCB hole diameter. Rectangular leads: find the lead diagonal ().
Then add 6 mils to get the recommended PCB hole diameter. ( 6 mils ≈ 0.15 mm
)[11][12]

voltage regulators and other components in TO-220 packages typically fit
in 0.040" (1 mm) holes. Some people prefer a "universal layout" that supports
practically any 3-pin regulator.[5]

DIP package ICs and TO-95 typically fit in 0.029″ diameter holes[5]
(0.8 mm diameter).[6]

"The component lead - hole clearance should be 0.4 mm" [13]

"The optimum pad diameter for a through-hole component is twice its
finished hole diameter."[14]

0.1" pitch pin headers from many manufacturers[7]
are typically 0.025 inch (0.64 mm) square. Manufacturers typically recommend a
hole 0.040 inch (1.00 mm) diameter.[8][9]

A tooling hole or mounting holes ... A "tooling hole" -- used to
temporarily attach the board to test fixtures, during assembly and test. They
are almost always 0.125" in diameter, unplated , and placed in opposite corners.
Two are required, but a third can prevent reverse installation of the PCB. It is
possible to use these as mounting holes for the end-use of the PCB.

Many manufacturers publish their "standard hole sizes" (standard drill bit
sizes minus the standard barrel thickness of through-hole metal plating). The
man running the drill press prefers to see standard sizes; otherwise he is
forced to either (a) pick the next-smaller standard drill bit -- then the
physical part won't fit in the hole; (b) pick the next-larger drill bit -- this
pushes the through-hole metal plating out, possibly hitting some internal trace
and rendering the entire board unusable; or (c) reject the board as
unmanufacturable. To avoid all 3 problems, often PCB designers "round up"
non-standard hole sizes to the next larger standard hole size -- i.e., often
holes for DIP packages are rounded up to 0.9 mm diameter -- and then run the DRC
check. If the DRC finds any traces that are now "too close" to the bigger hole,
the designer pushes those traces a safe distance away before sending the design
to the manufacturer.

Board Thickness
and Layers[edit]

The vast majority of PCBs have an overall thickness of 1/16 inch (1.58 mm).
Some very dense SMT boards have an overall thickness of 1/32 inch (0.79 mm),
which allows smaller via holes to be drilled, allowing denser packing.
Occasionally boards are made with an overall thickness of 3/32 inch (2.3 mm),
which makes it more rigid (but requires bigger via holes).

Often some or all layers are almost entirely covered with a "copper pour"
("ground plane" or "power plane"). Such pours typically have a signal-to-pour
clearance of 0.010 inch and clearance from the cut edge (perimeter of the board
edge) to pour of 0.020 inch[15].

(more layer stackup tips)

Most PCBs have between one and twenty conductive layers laminated (glued)
together in a sandwich with insulating plastic. PCBs with more than two layers
help construct complex or dense circuits. They are not always used because they
are more expensive, and the inner layers are more difficult to inspect and
repair.

In more complex PCBs, two or more of the layers are dedicated to providing
ground and power. These ground planes and power planes distribute
power well. They also prevent radio waves from antennas unintentionally formed
by tracks. These planes are rectangular sheets of foil that occupy entire layers
(except for small holes to avoid unwanted connection to vias and through-hole
components). They distribute electrical power and heat better than narrow
traces. Sometimes solid metal PCBs with thin layers of insulation are used. The
power electronic substrate carries away waste heat when air cooling is
impossible.

Four-layer PCBs with a ground and power plane are often used in high-quality,
but cost-conscious audio, avionics and medical electronics. Most consumer
products have one or two layers.

If you want to use a BGA-packaged part, that one part typically dictates the
number of layers the PCB must have. With a few low-density BGA packages, it's
possible to use a 2-layer PCB[10][11][12]
Some BGA packages require at least 4-layer PCBs, and many BGA packages force
designers to use even more PCB layers.[13][14][15][16][17][18]
For example, a BGA package with 7 or 8 rows of balls (from the center to the
perimeter) generally a minimum of 6 layers to fan-out, including a power plane
and a ground plane.[19][20]
Some BGA packages with over 1000 pins and a pin-pitch of 0.8 mm require at least
8 layers and blind, buried, and micro-vias.[21]

Often all the electronic parts of a system work fine with a 4-layer board or
even a 2-layer board except for one part in a BGA package. Rather than designing
one big full-custom 10-layer board to hold everything, many people prefer -- at
least for the first prototype -- to partition the design into two PCBs -- or
more. One board that that includes that BGA part -- often a commercial
off-the-shelf (COTS) board, preferably one that includes as much as possible of
the rest of the system -- and custom design a much simpler 2-layer or 4-layer
board(s) to support the remaining parts. Often there is a more-or-less
standardized interface -- carrier boards and stacking modules,[22]
FPGA Mezzanine Card (FMC)[23]
for I/O modules to connect to a FPGA; etc.[24]

Trace clearance[edit]

The width and spacing of conductors (or "traces") on a PCB is very important.
If the traces are too close, solder can short adjacent traces, and the PCB will
be difficult to construct or repair. If too far apart, the PCB may be too large
and expensive. When a PCB carries high frequencies, traces may need to be exact
widths and lengths to control the characteristic impedance of the trace.

The "clearance" is the shortest distance through the air between two
conductors. [25]
For mains-powered information technology equipment, UL 60950-1 gives the minimum
allowed PCB spacing. With typical 120-230 VAC mains input, creepage between
primary and low-voltage secondary circuitry per UL/IEC 60950 should be 6.4 mm
minimum. [26]
[27]
[28]
[29]
The IPC recommends a clearance between tracks of 0.0254 mm/V on uncoated boards
expected to ever be used above 10,000 ft, 0.005 mm/V on uncoated boards expected
to always stay below 10,000 feet, and 0.00305 mm/V between traces under a solder
mask. Some safety standards require a minimum of 8 mm clearance between mains
input (240 V) and signal tracks. [30]
[31]
Other standards related to clearance and creepage include ECMA 287, IEC 60664,
NEMA 1-111-1, NEMA 1-111-2, etc.

Some designs cut the ground plane or the entire PCB in strategic locations to
control the return paths of currents. The usual desire is to keep high voltages
or frequencies away from sensitive portions of a circuit. The actual properties
of the design are critical, because in some cases, cutting the ground plane
makes the PCB into an antenna that radiates radio noise into nearby
equipment.

Remove less
copper[edit]

Removing large areas of copper wastes etchant and can increases waste
(although commercial fabricators reclaim the copper and regenerate the etchant).
Also, a PCB etches more consistently and tends to resist warping if all regions
have the same average ratio of copper to bare board. Therefore, designers may
widen connectors, leave unconnected copper in place, or cover large areas of
what would otherwise be bare board with arrays of small, electrically isolated
copper diamonds or squares.

Fiducial[edit]

Most PCBs have alignment marks (called fiducials) and tooling holes to align
layers.

The preferred fiducial is a solid circle 1 mm diameter.[32][33][34][35][36][37][38][39]
These permit the PCB to be mounted in equipment that automatically places and
solders components. Some designs also have quality control patterns to measure
soldering and etching processes. In some cases, the test patterns are on
break-off tabs that can be removed before the PCB is installed.

Via[edit]

Layers may be connected together through drilled holes called vias.
Either the holes are electroplated or small rivets are inserted. High-density
PCBs may have blind vias, which are visible only on one surface, or
buried vias, which are visible on neither, but these are expensive to
build and difficult or impossible to inspect after manufacture. Good designers
minimize the number of vias to reduce the cost of drilling. On older, two-layer
PCBs, it was common to solder a wire through the hole.

Solder mask and
silkscreen[edit]

Wikipedia has related
information at reference
designator#Reference designations

A solder mask is a plastic layer that resists wetting by solder (the solder
is said to "bead up"), and keeps islands of solder from running together. It
also protects the outside conductors layers from abrasion and corrosion. Without
the solder mask, the fibreglass-reinforced epoxy appears a translucent
off-white. Solder masks are usually green, but they may be found in other
colours.

A silkscreen legend on the top or bottom surface of the board provides
readable information about component part numbers and placement. This aids in
manufacturing and repair. To aid manual construction and repair, diodes,
capacitors and integrated circuits are sometimes oriented in the same
direction.

New technology allows for the component designators to be printed directly
onto the board surface, saving time and money by doing away with silkscreens.
This is sometimes done by a special inkjet printer. A similar process has
experimentally produced solder masks.

Basic guidelines[edit]

Radio transmitters and radio receivers are difficult to design. PCB designers
working on them must minimize parasitic effects due to layout of components, or
take them into account with a general model and use simulation software
such as SPICE.

Fortunately, many practical circuits can be laid out using a much simpler
lumped element model.

PCB layout Basic guidelines:

it is often a good idea to have made a prototype circuit using
point-to-point construction or wire wrap, as you will have solved certain
basic issues to do with component selection: (e.g., should I use a 1/4 watt
resistor here, or do I need 1/2 watt?)

consider physical constraints on the assembled board's size and heat
dissipation requirements; choose your heat sinks if needed.

consider carefully the physical size of the components you are laying out;
the circuit schematic doesn't tell you this. Equivalent components often have
different packages.

How do the components attach to the board? Are they surface mount
components? or do they require holes, screws, washers, etc.?

are there mechanical parts directly mounted to the board? For example,
switches or variable resistors?

How will the board mount in its container? What stresses (shock, strain,
shear) will there be upon it and upon components?

How will the board connect to its power source? What other connectors will
be required (e.g., signal inputs, outputs)?

use construction paper and a pencil and sketch the board in its actual
size; or use component layout software that includes information about the
component outlines.

decide appropriate widths for each of the signal traces; this depends on
the current each trace is expected to carry.

decide whether you will have a single-layer board, 2-layer, or multi-layer
based on the circuit complexity and fabrication costs.

begin by placing component outlines, then by placing signal traces; leave
a little room around each for tolerances.

for a single layer board, spend more effort to avoid having traces cross
each other; play with component placement or run traces underneath components;
sometimes a jumper wire is needed.

in 2-layer and multilayer boards simply run the traces on different
layers, and use plated-through holes to jump from one layer to another.

try to predict and avoid assembly errors: where there are multiple
components of the same kind, or where pins have a polarity (e.g., electrolytic
capacitors), try to place them in parallel and orient the positive pin in the
same direction.

If your PWB design software has a DRC (design rule check), use it.

PCB layout guidelines for RF circuits on a 2-layer or multilayer
board:

identify the critical parts of the circuit and lay them out first

have one of the layers act as a continuous ground plane.

if signal traces are constant width and height above the ground plane, and
are properly terminated, then their characteristic impedance is more
well-behaved and may be calculated.

avoid sharp corners.

keep signal traces and component leads as short as possible.

inputs and outputs should be far apart, so that RF energy will not leak
back from output to input. stages should line up, rather than snake
around.

decouple the RF parts of the circuit from the DC parts of the
circuit.

shield AF and IF components from RF components.

high-speed communication (over 100 Mb/s per wire) generally requires
point-to-point connections, rather than multi-point multi-drop bus
connections. Communication over 622 Mb/s per wire requires even more
specialized techniques and careful connector selection.[40]

Many people have a checklist of things to review before sending the Gerber
layout files to the PCB fabricator.[41][42][43][44][45][46][47][48][49]

Further Reading[edit]

Wikipedia
has more about this subject:

design
for manufacturability

Wikipedia
has more about this subject:

design
for manufacturability (PCB)

How
To Be A Circuit Board Designer (tutorial)

Chip
Design Made Easy describes some issues that effect both chip designers and
PCB designers, such as EMI.

Robotics:_Design_Basics:_Design_software#Schematic_Capture_.26_PCB

Wikipedia:
schematic capture

Wikipedia:
electronics

Wikipedia:
electronics manufacturing

Wikipedia:
electromagnetic interference

Wikipedia:
circuit design

Wikipedia:
schematic

Wikipedia:
printed circuit board

Wikipedia:
Gerber format

Wikipedia:
ground plane and Wikipedia:
power plane

Wikipedia:
power electronic substrate

Wikipedia:
characteristic impedance

Wikipedia:
fiducial

Wikipedia:
SPICE

Wikipedia:
electrical network

Wikipedia:
lumped element model

Wikipedia:
point-to-point construction

Wikipedia:
wire wrap

some components require Wikipedia:
heat sinks for heat dissipation

Wikipedia:
surface-mount technology

Wikipedia:
signal trace

Wikipedia:
electric current

Wikipedia:
electrolytic capacitor

Wikipedia:
electrical termination

Wikipedia:de:Leiterplattenentflechtung

References[edit]

↑
Standard PCB Layout Process Flow (911EDA)

↑
National Semiconductor knowledge base: "What is the translation
between PCB copper thickness in ounces, inches, and mm?"

↑
Screaming Circuits: "LED and diode markation
guidelines"

↑
Diversified Systems: "Production electronic assembly layout
guidelines: Designating polarity"

↑ a
b
David Cook. "PCB Layout Tips".

↑
"Drill sizes"

↑
Wikipedia: pin
header

↑
"3M Pin Strip Header, 961 Series"

↑
"Molex KK 254 header"

↑
Abhay Nadkarni. [http://
www.cypress.com/?docID=25208 AN43841 "56-Ball BGA PCB Layout
Guidelines"]

↑
"http://www.altera.com/literature/an/an114.pdf"

↑
2-layer BGA PCB

↑
"General hardware design/BGA PCB design"

↑
"PCB Layout Recommendations for BGA Packages" Lattice
Technical Note TN1074. [1]

↑
Lattice. "Low cost board layout techniques for designing with PLDs in
BGA packages"

↑
"Escape routing under fine pitched BGAs."

↑
"Four- and Six-Layer, High-Speed PCB Design for the Spartan-3E
FT256 BGA Package"

↑
"How many layers needed for 1000 pin bga"

↑
Section 5.2: "How many PCB layers to fan-out the
BGA", from "NXP AN10778: PCB layout guidelines for NXP MCUs in BGA
packages"

↑
Abhay Maheshwari and Soon-Shin Chee. "Board
Routability Guidelines with Xilinx Fine-Pitch BGA Packages"

↑
Charles Pfeil. "BGA Breakout Challenges"

↑
Robotics/Computer
Control/The Interface/SBC and multichip modules#Stacking modular connector
boards

↑
Wikipedia:
FMC – FPGA Mezzanine Card

↑
"custom FPGA PCB Design tips".

↑
"Creepage and clearance distances" [2]

↑
"The basics of PCB (printed circuit board)
layout: guidelines for switching power supplies (SMPS) design" [3]

↑
"Spacing between PCB traces for various voltage
levels: circuit board layout guidelines" [4]

↑
Clearance Calculator and Creepage Calculator [5]

↑
Milton Hilliard. "PCB Layout: The Impact of
Lightning and Power-Cross Transients". Compliance Engineering 2003. [6]

↑
"PCB Design Layout Rules Recommendation" [7]

↑
IPC2221 section 6.3 [8]

↑
"PCB Design Tutorial" by David L. Jones. "The fiducial mark
should be a circular pad on the copper layer of diameter 1.5mm"

↑
"Fiducial Mark Design Guidelines" "Some say that the
optimal fiducial mark is a solid filled circle. ... The minimum diameter of
the fiducial mark should be 1 mm (0.040 in)."

↑
"CPI Electronics: Manufacturing Design Guidelines"
"Fiducial Mark: A 1 mm (+/- 0.1) circle or 2 mm (+/- 0.1) cross is the
preferred pattern."

↑
"Centroids and Fiducials" "please make sure your fiducials
are a minimum 1 mm center pad diameter."

↑
Dynatech: "Samsung SMP200 Screen Printer" "Fiducial Size:
0.020~0.157" (0.5~4.0mm)"

↑
Tracktronics: "Pick and Place Fiducial Requirements"
"Smallest size of any fiducial mark is 0.5mm. Recommended size is 0.75mm. The
recommended shape is a circle, followed by square, then cross
hair."

↑
South Bay Circuits: "Manufacturability Guidelines For Printed
Circuit Board Assemblies" "The Surface Mount Equipment Manufacturers
Association (SMEMA) has standardized on design rules for fiducials. These
rules are supported by the IPC and adopted by SBC ... The optimum fiducial is
a solid filled circle. ... Size: The ... diameter of the fiducial mark ...
0.040” ... 1 mm is preferred. Fiducial marks should not vary in size on the
same PCB more than 0.001” (0.025mm)"

↑
Acme PCB Assembly: "Fiducial mark requirement" "The shape
of the Fiducial shall be a solid filled circle. The minimum diameter of the
Fiducial Mark shall be 1.00 mm [0.040 inch]."

↑
Lattice Technical Note TN1033 "High-Speed PCB Design
Considerations"

↑
Xilinx PCB Design Checklist

↑
"Steve’s PCB layout checklist"

↑
"standard PCB documentation file": a list of diagrams and
"source" files that contain all the information required to fabricate or
further develop the product.

↑
[9]

↑
"Golden Rules For Preventing Parts Headaches At PCB
Layout"

↑
http://www.volersystems.com/v-2010-issue-1/pcb-layout-checklist
Voler Systems "PCB Layout Checklist", based on Hank Wallace: "Electronics Design Checklist"

↑
http://www.adcom.co.il/engineering/pcb_chl.htm Adcom: "PCB
layout checklist"

↑
"Intel® PXA27x Processor Family Design Check List" section 4.0
"PCB Layout Check List"

↑
"PCB Layout Checklist"

External links[edit]

Wikipedia
has more about this subject:

printed circuit
board

Wikipedia
has more about this subject:

electromagnetic
compatibility

Retrieved from "https://en.wikibooks.org/w/index.php?title=Practical_Electronics/PCB_Layout&oldid=2959540"

Category:

Practical
Electronics

Navigation menu

Personal tools

Create
account

Log
in

Namespaces

Book

Discussion

Variants

Views

Read

Edit

View
history

More

Search

Navigation

Main
Page

Help

Browse
wiki

Cookbook

Wikijunior

Featured
books

Recent
changes

Donations

Random
book

Using
Wikibooks

Community

Reading
room

Community
portal

Bulletin
Board

Help
out!

Policies
and guidelines

Contact
us

Tools

What
links here

Related
changes

Upload
file

Special
pages

Permanent
link

Page
information

Cite
this page

In other languages

Čeština

Add
links

Sister projects

Wikipedia

Wikiversity

Wiktionary

Wikiquote

Wikisource

Wikinews

Wikivoyage

Commons

Wikidata

Print/export

Create
a collection

Download
as PDF

Printable
version

This page was last modified on 18 May 2015, at
12:34.

Text is available under the Creative
Commons Attribution-ShareAlike License.; additional terms may apply. By
using this site, you agree to the Terms
of Use and Privacy
Policy.

Privacy
policy

About
Wikibooks

Disclaimers

Developers

Mobile
view