CALCULATING SPACING BETWEEN PCB TRACES FOR VARIOUS VOLTAGE LEVELS

CIRCUIT BOARD LAYOUT GUIDELINES

Proper
distances between PCB traces are critical to avoid flashover or tracking between
electrical conductors. Unfortunately, there is no single solution to this issue.
There is a variety of industry and safety standards that prescribe different
spacing requirements depending on the voltage, application and other factors.
Here I am providing some considerations and a simple widget that will help you
determine the proper spaces between PCB tracks.

Home

Tutorial

Topologies

SMPS
design

Software

PCB
design

Computer PSU

UPS

Circuit

Transformers

Formulas

EE
Reference

Inverters

Thermal
design

Generators

Solar

SAFETY REQUIREMENTS

When a product has to be recognized by a
certain safety agency, there may be a legal requirement to meet specific
insulations listed in the relevant agency's standard. In this case, finding the
required spacing is more or less straightforward. For example, in the U.S. for
most mains-powered or battery-powered information technology equipment, the
minimum allowed PCB spacing should be determined from UL 60950-1 2nd
Edition Tables 2K, 2L, 2M or 2N. These tables specify so-called clearance
and "creepage" distances for various grades of insulation as functions of
working voltage, pollution degree, PCB material group and coating.

The required grade depends on the location of the circuit. The
standard specifies functional, basic, supplementary, double and reinforced
insulations. For example, when a breakdown can create a hazardous voltage on
user accessible conductive parts (such as in case of insulation between mains
circuits and low-voltage secondary circuits), a double or reinforced insulation
is required. In this case, to separate such circuits on the PCB you need to
double the respective distances shown in an appropriate table. The diagram below
illustrates the clearance and creepage measurements and lists the requirements
(in mm) for a typical application when both mains and working voltages are under
300VAC. Note that 1 mm ≈ 40 mils. If you don't have an access to the UL
document, this creepage calculator will help
you find the necessary distance. Of course, you should consult with UL 60950-1
or an applicable standard for final design decisions. Note that for the
equipment manufactured in China and intended for use at altitudes above 2,000m
(up to 5,000m), according to GB 4943.1-2011 the minimum distances has to be
multiplied by 1.48.

OPERATIONAL REQUIREMENTS

The
distances provided by IEC and UL actually greatly exceed the spacing necessary
for proper operation of the devices. This was done in order to provide increased
protection against electric shock. For the circuits whose locations do not
require electric shock protection, spacing between printed circuit tracks can be
made smaller.

For the so called functional insulation,
UL 60950-1 permits to use separation distances lesser than the specified in
their charts. They just have to withstand the electric strength test (casually
called Hipot) per Par.5.2.2 Table 5B. In other words, where
only functional insulation is required, you don't need to meet any specific
clearance between PC traces for as long as there will be no electric breakdown
between them at the prescribed test voltage. The latter generally is several
times greater than actual working voltage between separated traces.
Unfortunately, there is no clear information in the literature on what is actual
breakdown voltage between the conductors and how to design a PCB to pass a
specific hipot. Experiments performed by UL in the course of analysis of
silver PCB surface finish, demonstrated that the withstand voltage of a pair of
parallel conductors is purely a function of the spacing, not surface finish.
Based on the experiments, UL specified withstand voltage of 40 volts/mil
or about 1.6 kV/mm in their UL796 Standard for Printed Wiring Boards. In my
view, it is reasonable therefore to use these numbers in designing the board to
withstand a particular test. For example, for working voltage 500V in secondary
circuits you need to withstand 1740 Vrms per UL 60950-1 Table 5B Part 2. Such
sinewave has 1740*√2=2461 V peak value. With the 40V/mil criterion, the required
minimum spacing would be 2461/40=62 mils (or 1.6 mm).

Voltage (DC or AC peak)

SPACING

mm

inches

IPC-2221B:

external

internal

coated

IPC9592

For products that are not covered by UL60950-1 safety standard, to
determine the electrical clearances the designers normally consult with
IPC-2221. It is widely accepted throughout the world as a generic PCB design
standard for commercial and industrial applications. The Table
6.1 of IPC-2221A specifies minimum required conductor clearances as a
function of voltage, elevation level and the coating. Since their introduction
in 1998, these numbers were never revised. IPC just added the values in inches
in revision A and left them unchanged in rev.B.
Of course, it is always
desirable to maximize whenever possible the distance between tracks on
individual layers to minimize the possibility of electric breakdown and reduce
parasitic capacitance. However, because of usual shortage of space on a PCB,
spreading out the traces and components more than it is really necessary may not
be feasible. From a technical standpoint, IPC stepwise clearance limits are
mostly baseless. For example, there is no reason whatsoever, why you need 2.5mm
for 301V, while for 300V you can use 1.25mm. A recent IPC-9592 standard
for power conversion circuits originally provided linear functional spacing
requirements: SPACING (mm) = 0.6+Vpeak×0.005. Linear function of course
makes more sense. However, in most cases the above formula resulted in even
higher spacings and in grossly over-designed circuit board. Later revisions of
this document returned to a sort of step function and relaxed the requirements
at the low end: 0.13mm for V<15V, 0.25mm for 15V≤V<30V and
0.1+V×0.01 for 30V≤V<100V. Our widget provides rounded numbers based
on the above equations.

One would think that a general standard has to
be more liberal than UL requirements. In reality, for V>150V IPC actually
calls for larger spacings between uncoated external conductors than those you
can derive from UL 60950-1 Table 5B in conjunction with the 40V/mil criterion.
Note that generally all IPC doc's are voluntarily rather then mandatory.
Particularly, they state that "Existence of such Standards and Publications
shall not in any respect preclude any member or nonmember of IPC from
manufacturing or selling products not conforming to such Standards and
Publication".

Where shortage of space on a PCB is an issue, for non-UL
applications you may need to use the spacing smaller than those that are
prescribed by IPC. However, be sure to use an ample safety factor to withstand
the voltages substantially higher than the peak voltage between the traces under
any abnormal and transient conditions. It is interesting to note that many major
power supply manufacturers in their low-power off-line designs are widely using
500-800V MOSFETs in TO220 package operating at 400V and higher. With this
package you can get about 30 mils spacing between the pads, while the documents
would require at least 100 mils. Even if you spread the leads on the PWB, you
can't do anything with 50-mil spacing between the TO220 leads along the surface
of the package.

As a reference, the chart below compares PCB distance
limits based on the following three specs:

IPC2221A for external layers for uncoated bare board;

IPC9592B;

UL60950 for functional insulation in secondaries, designed to meet the
test per Table 5B with the assumption of 40V/mil withstand voltage.

Note the curves below are for functional (not safety!)
insulation.

CONCLUSION

When the product is covered by an UL standard, you need
to select the appropriate table in the UL standard. Particularly, for the
products covered by UL60950-1, determine the grade of insulation depending on
the location of the circuits and then find from Tables 2K-2N minimum required
spacing based on working voltage, pollution degree, PCB material group and the
coating. For functional insulation UL permits usage of lesser distance if it
withstands the test voltage per Table 5B. For practical purposes, in my view,
you can calculate the distance on the assumption that the circuit board
withstands 40V/mil (1.6kV/mm). Of course, this test voltage is always much
higher than actual operating voltage. Also note that technically the insulation
requirements given in UL 60950 are for frequencies up to 30 kHz. So far,
60950-1 2nd Edition permits to use the same requirements for frequencies above
30 kHz until they will figure out what to do about it. You can't rule out that
in the future UL would adopt tougher standards for high frequency circuits based
on IEC 60664-1 and IEC 60664-4, which would have a major effect on most SMPS
designs.

If there is no legal requirement to meet UL or any other product
control law, try to use IPC-2221B (or IPC-9592B for power circuits) distance
recommendations whenever possible. However, where shortage of space on a PCB is
an issue, you may need to choose a smaller spacing, provided it still withstands
test voltages substantially higher than the peak voltage between the traces. The
above analysis takes into account only electrical breakdown issue. There are
other criteria that should be considered when selecting electrical clearance,
such as conductor's temperature
rise. Also see general guidelines for printed circuit board design, layout
rules for power circuits, and signal integrity issues.

Legal: The information provided here reflects only a personal
opinion of the author and does not constitute a professional or legal advice. It
is not intended to substitute official standards-- consulted them for all final
decisions. Also see our general Disclaimer linked below.

Material
Connections Disclosure | Disclaimer and Terms Of Use | Contact Information | About | Privacy

©2009, 2014 Lazar Rozenblat