The distances provided in UL 60950-1 actually greatly exceed the spacing necessary for proper operation of circuits. 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 varies depending on the working voltage and generally is several times greater then 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 meet a specific withstanding test voltage between the tracks. 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 test methods of 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 HiPot. For example, for working voltage 500V you need to withstand 1740 Vrms per UL 60950-1 Table 5B. Such sinewave has 1740*√2=2461 V peak value. With the 40V/mils 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 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 electrical conductor clearance as a function of voltage, elevation level and the coating. One would think that a general standard has to be more liberal than UL requirements. In reality, for voltages above 150V level, IPC actually calls for larger spacing between uncoated external conductors then those you can derive from UL 60950-1 Table 5B in conjunction with the 40V/mil HiPot criterion. Of course, it is always desirable to maximize whenever possible the distance between conductors
on individual layers. This is done in order to minimize the possibility of electric breakdown and to 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-2221 stepwise clearance limits are mostly baseless. For example, there is no reason whatsoever, why you need 2.5mm clearance for 301V, while for 300V you can use 1.25mm. A recent IPC-9592
standard for power conversion circuits provides linear functional spacing requirements: SPACING (mm) = 0.6+Vpeak×0.005. Linear function makes more sense. However, in most cases the above formula results in even higher spacings than IPC 2221 and in grossely overdesigned circuit board. Note that generally all IPC doc's are voluntarily rather then mandatory. Particularly, IPC-2221 states 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 then 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 IPC would require at least 100 mils. Even if you spread the leads on the PCB, 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 clearance limits based on the following three specs:
- IPC2221 for external layers for uncoated bare board;
- UL60950 for functional insulation, designed to meet HiPot 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 a 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, UL 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-2221A (or IPC-9592 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 the guidelines for printed circuit board design
for power circuits.
: The information provided here reflects only a personal opinion of the author and does not constitute any professional or legal advice. For final decisions consult the appropriate standards. Also see our general Disclaimer linked below.