3
\$\begingroup\$

Why does the IPC standard allow for smaller clearance on inner layers than external layers?

In this thread it is alleged that external layers are susceptible contamination. That makes sense with home-etched boards. But I thought no contaminants could get to the copper layers through the solder-mask.

For example, the IPC: IPC2221A (mentioned in that same thread) recommends for 100V traces a minimum clearance of only 0.2mm for inner layers, but 0.4mm for external coated layers.

Does it have to do with the conductivity of the PCB itself or the solder-mask?

\$\endgroup\$
1
  • \$\begingroup\$ Solder mask is not an environmental protection system.. there are gaps to allow soldering...and contamination. \$\endgroup\$ – Spoon Sep 29 '16 at 19:33
3
\$\begingroup\$

A good quality shop can support track and gaps on any layer of;

  • 3 mil (0.12mm) in std quality and
  • 2 mil (0.08mm) on advanced ($) build.

So it is not a process limitation but a contaminant limitation on the effect of breakdown voltages.

Here inner layers can be contaminated by air voids which cause a lower dielectric constant of air 1 vs FR4 >=4. This results in a higher E field and charge buildup in a void which can cause early breakdown.

We call it Partial Discharge (PD) and it behaves like a injunction oscillator, until more rapid and external then it is called corona.

Even though FR4 is rated >=500V per 0.1mm a, void can breakdown in about 1/4 of this. Since a full breakdown voltage thru the dielectric between high voltage conductors is usually followed by extreme high current from storage capacitance of low impedance AC sources, I believe IPC has implemented at least a 2:1 safety factor for internal gaps between HV conductors.

For the outer surfaces it is worse. Even though the solder mask is an excellent insulator like FR4 epoxy, the surface can be bridged by dust and humidity and creates partial discharges that lead to a full breakdown depending on then thickness of dust, humidity and salt spray so,even more safety margin is required for dielectric breakdown on the surface which is equivalent to 100V/0.4mm or 250V/mm about 1/10th of the breakdown of flat surfaces in clean air or 1/4 of sharp edges in clean air..

The key requirement here is safety and flammability under high voltage follow on current. If one is designing a custom board for microcurrent HV levels and has a somewhat sealed environment, they may deviate from the said IPC guidelines. But dust and humidity as well as epoxy voids both degrade the arc flash thresholds of clean pure dielectrics.

\$\endgroup\$
0
3
\$\begingroup\$

External layers are plated-up with additional copper after etching, whereas internal layers usually aren't. This can lead to larger manufacturing tolerances, though one could argue that it's the board house's responsibility to deal with that rather than the IPC standard.

Also, solder mask has deliberate openings, some registration tolerance (which can be significant) and isn't immune to damage. Its thickness may not be especially well controlled and it does not have guaranteed dielectric performance, whereas the core or prepreg material surrounding the traces on inner layers does. The primary purpose of solder mask is to aid soldering yield - the insulation and mechanically protective qualities are secondary. Where those qualities are critical it would be better to use a conformal coat.

\$\endgroup\$
1
  • 1
    \$\begingroup\$ Layer of board is a known dielectric. Soldermask is not... \$\endgroup\$ – Ecnerwal Sep 29 '16 at 19:53

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.