next topic »

[on:]

I find all kinds of things on the web when trying to figure out the minimum clearance to 220 VAC on a PCB.  This relay from Sparkfun is made for 220VAC:
https://www.sparkfun.com/products/10924

If I add this relay to my eagle design using their footprint, the clearance between the two output pins is 4mm.  So if it's only 4mm there, I don't need to have 8mm (like one site suggested) everywhere else.  (I'm tight on space or I'd be happy to put lots of clearance)  I just don't want to make something too unsafe.
thanks.

[Reply #1 on:]

How are you planning to connect the relay? If you have the 220V supply going to the common contact and one or both of the other contacts connected to devices to be powered, then if the worst happens and a large mains transient causes a discharge between the two pins, all that will happen is that the transient will reach the device that is supposed to be off. Depending on the application, this very likely doesn't matter.

It's much more important to maintain the 8mm clearance between the 220V pins and the relay coil pins/all the other non-mains circuitry on your PCB/anything the user might be able to touch.

[Reply #2 on:]

People normally cut a slot in the PCB as well as using a minimum clearance (otherwise moisure/dirt/ants can cause tracking and flashover). 

Make the space as large as possible (4mm is not adequate for a safety critical isolation).  An alternative is potting
the back of the PCB in silicone (electrically rated, not bathroom!), excluding moisture, insects and fingers all in
one go.

220Vac can have multi-kV spikes on it in real life (fridge motors with failed snubber, lightning strikes), so this is why a large
clearance is required.

[Reply #3 on:]

You have to clear all the copper over your mains to if using a double side board

[Reply #4 on:]

You have to clear all the copper over your mains to if using a double side board

...so the board isn't enough of an insulator for 220VAC?

[Reply #5 on:]

You have to clear all the copper over your mains to if using a double side board

...so the board isn't enough of an insulator for 220VAC?

The board is not as thick as the minimum gap so yes you have to do it. It is also capable of coupling high voltages into the ground plane as it acts as a capacitor.
The slots used in PCBs are to get stuff closer. The rules on air gaps are different from the rules on PCB spacingq.

[Reply #6 on:]

You have to clear all the copper over your mains to if using a double side board

...so the board isn't enough of an insulator for 220VAC?

Probably yes, since the dielectric strength of NEMA-standard FR4 is 14kv/mm minimum. However, you would need to be certain that your board meets the NEMA standard, and you need to allow much more than 220V strength to allow for mains transients. Also, you would need to keep the copper well clear of the edges of the board, on order to meet the creepage specification. It's simpler to remove the copper from the area underneath the mains wiring traces.

[Reply #7 on:]

...so the board isn't enough of an insulator for 220VAC?

The thing you must understand is that this is not about being safe it is about meeting safety requirements. The two are totally different things. Some safety requirements are total over kill ( maybe kill is the wrong word with safety ) some things that meet safety requirements can be a bit iffy.

[Reply #8 on:]

dc42 if you need more then 2.5 mm the board is 1.4 to 1.6 thick I would remove the copper. And as a side note I have not seen any board that didn't have the copper remove from one side with high voltage below.

So your saying cut back the side copper to get it like remove 2mm around the edge of the board

This is what I would use    

[Reply #9 on:]

Some folks here seem to be confusing insulation thickness with creepage specification. Your insulation specification may call for 8mm minimum separation for creepage, meaning that the shortest path between the conductors concerned along the surface of the PCB and/or the surface of the components must be at least 8mm. But that does not mean you need 8mm think insulation. So a PCB much thinner than 8mm can meet the requirements, in principle. You would still need to remove the copper within about 4mm of the edges of the board on each side to meet the creepage requirements.

But why bother going to the trouble of getting your PCB quality-controlled for thickness and dielectric strength and insulation tested, and having an extra certification hurdle to jump, when it is much easier to remove the copper from the other side of the board under the mains traces?

As an example of meeting requirements using thin insulation, the ADUM6401 series of digital isolators achieve 5kV RMS UL 1577 isolation with just 0.017mm thick (minimum) insulation (and 8mm creepage clearance across the package).

[Reply #10 on:]

Here a picture of that relay mounted on the back side showing the copper

[Reply #11 on:]

So if it's only 4mm there, I don't need to have 8mm (like one site suggested) everywhere else.

There are industrial safety standards that specify clearances on 220 VAC traces, etc. If you
want to be safe, you might do well to specifically look that up, rather than relying on "like
one site suggested".

[Reply #12 on:]

This board can have 120 VAC up to 30 A running thru it.
http://www.pololu.com/catalog/product/1187

http://www.pololu.com/file/download/ACS714-Datasheet.pdf?file_id=0J196

Looking at a SOO8 package in Eagle I see the pins are 1.27 mm apart, so I'm guessing the clearance between the traces of the AC in and out must be about 1 mm.  That's way below the isolation range, isn't it? 

[Reply #13 on:]

Well they must not of trusted it or the Crimp Terminals would be yellow not blue LOL

2.1 kVRMS minimum isolation voltage from pins 1-4 to pins 5-8

[Reply #14 on:]

Well they must not of trusted it or the Crimp Terminals would be yellow not blue LOL

This went over my head!?

In your picture, for 250 V it shows a clearance of (1.25, 6.4, & 0.4) for External conductors uncoated, uncoated >3050m, and coated.
What's the difference between uncoated and uncoated >3050?  I get my boards from BatchPCB, they have a solder mask on them, but somehow I don't think that qualifies me to have 250V traces only 0.4 apart! 
Bottom line is:  I remove all copper from other side of board, I'll use the largest value there, which is 6.4mm clearance between traces.  Then I should be good?  (I still don't know how they can have 2 pins next to each other on an SOO8 package having large voltages on them...