I used to repair cordless phones and modems that had died after a lightning surge (major issue in Malaysia)
It was always the opto hook switch relay flashed over.
Yes. I have had power supplies with optocoupler feedback become VERY NOISY…garbage operation… when they needed to have the isolation barrier bypassed with one or two nF. I think that the added capacitors suppress rapid common mode voltage spikes from the switch node and coupled by transformer capacitance.
Hello, just for fun:
I have a very old proposel from a magazine to build a custom optocoupler by combining a black plastic tube with a (IR)LED and a phototransistor. Even the phototransistor was “handmade” by opening a TO18 standard transistor !
This way one can achieve ANY safety distance 
It’s not clear to me how much additional creepage distance can be obtained with a slot. The part itself has a creepage distance that isn’t much more than the pin to pin spacing. So how do you mill a slot in the part package?
Is there something special about the package that withstands voltage creeping across the surface than a PCB does?
Creepage over the package is not a straight line of the width, but it goes up and down over the package. The thickness of a standard DIP8 is around 3.3mm and this is quite significant.
Creepage over the PCB is a straight line because the PCB is flat. It is further reduced by the amount that the pads extend on the “inside” towards each other.
1 Like
In my case I’m more worried about transients than high voltage leakage. However giving leakage more thought, I would think the extra opening will allow better cleaning.
Adding a slot in the PCB where the volts/cm is high really helps.
Another option is to add silkscreen over the area. Some time I cover the entire area and some times I make many thin lines to make the surface bumpy. This causes the electrons to travel further to get from point A to B. I tested this with my HV power supply and it works better.
In the picture there are three spots with 1500 volts. The silkscreen also helps me remember to keep traces out of that area.
The concern with this is the typical thickness of a silkscreen print is 15um, and thus 5 such printing patterns only increases the creepage distance by 0.15mm, not that significant. Now if thicker silk was used sure, but not bog standard fab house stuff
1 Like
Silkscreen is not designed for electric isolation, and can not be relied upon for such. Silkscreen is often printed with a dot matrix printer, and there may be small holes or other artifacts that prevent a decent form of isolation.
If you want extra isolation, add a decent layer of conformal coating, or use some potting compound.
The cheapest and easiest I can think of is a few mm of hot glue.
2 Likes
yup, slots, conformal coating or some bonded barrier (yup hot-glue would do, although I would use some former and bond it with DP-760 but the same principal).
As I always tell my engineers, over-current is a time thing, but over-voltage? do not pass go, go straight to avalaunch. It is the one thing when pushed by mechanical to “make things smaller” I do not budge…
1 Like
I hear what you say. I did test with a “hi pot tester” and a 10kV power supply.
A bear PCB with no solder mask performs poorly. Just adding solder mask increases the breakdown voltage far more than what 15um would account for. Adding silk screen increases the breakdown again.
Back in the “through hole” days I put silk screen under all resistors with high voltage on them. Electrons will break through the side of resistors and head for the nearest copper. I don’t think adding micro meters made the difference. It was adding another layer of insulation. Those resistors only had paint for insulation. I did not measure but adding a layer of “paint” to the PCB probably doubled the break down voltage.
Adding that silk screen is likely to have some effect, but that is not the point here.
It may help for hobby purposes, but for production you can not guarantee that each and every PCB will have it’s isolation boosted effective enough with a bit of silk screen, and therefore it can not be relied upon. For a reliable process, you need [Edit: A suitable] conformal coating.
1 Like
And with a specified / controlled breakdown voltage characteristic. I was in Automotive and was of the belief that if you made a million of anything you will find or get bit by anything that is not controlled. And often those that are controlled.
Factories hate conformal coating. Cost money and the repair department really hates it.
For high end test equipment we coat the boards. (some times)
For TVs and Monitors we never did. If the board is vertical condensation is not a problem. Horizontal mounted boards can pool water and spark over. We used slots, and/or silkscreen. I have had a number of call from Japan, Korea, Singapore where they removed the silkscreen in the HV areas because they did not know.
No argument, the coating is better. The silks cost me nothing, and the repair department does not threaten strike. lol
This thread has been wondering a bit off topic.
All these extreme measures are not really needed to get some decent clearance for just mains voltage rated PCB’s. For those it’s usually just assign some space to keep wide enough clearances, and maybe a few isolation slots, especially if heavy contamination levels are expected.
But you should never suck numbers for these out of your thumb. There are regulations for these, and if you want to make a compliant PCB, then make sure you adhere to these regulations.
A point I didn’t read here is to use rounded pads or pads with rounded corners to reduce field strength.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.