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.
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.
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.
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).
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;
- 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.
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
rules for power circuits, and signal integrity issues
: 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.