Creepage and clearance

[ricko_uk]

Hi,
I am routing a mains PCB with 250V traces spread all around it. It goes without saying that safety if by far the top priority so to get the right creepage and clearance is essential, but at the same time space is limited so I don't want to overdo the clearances over what is required to ensure proper safety.

A screenshot of a creepage and clearance table is attached. No idea which column I should consider for a residential electrical cupboard application.

1) Can someone please explain which column I should consider and why
2) what is the difference between reinforced and the others?
3) if more than one option, what is the safest "standard" to choose and which is the best/recommended?

Many thanks

[TimNJ]

IPC guidelines are generally very conservative. As far as safety standards are concerned, if you can ensure the board will be contamination free, you can use the following guidelines. These are derived from IEC60950/IEC60601. You can apply these for creepage and clearance, as a starting point. If you are in a bind, certain items can be met by adding a slot to increase creepage.

1. Between line and neutral, before fuse: >3mm
2. Between line and neutral, after fuse: >2 or 2.5mm. (Not really regulated as far as I know. I like to shoot for about 2.5mm minimum.)
2. Between two fuse leads (of the same fuse), on either line or neutral: >3mm
3. Between line/neutral and earth: >4mm
4. Between primary and secondary, or between non-isolated and isolated side: >8mm

[ricko_uk]

Thank you

Couple of more quesitons:

1) About the 8mm (point 4 above) is that also between two sides of a optocoupler where one side is mains and the other is isolated 3V3?
I cannot find an optocouplers with 8mm gap between the two sides and most of them are 4mm and they are rated at few kV. How does that work?

2) Also what are the rules and regulations for the same application if I want to place components with high voltage difference (275Vac)on top of each other on opposite sides of the PCB? For example:
- live trace on top and neutral trace on the bottom or
- either or the mains traces on top and 3V3 isolated on the bottom
Can I do that?

Thank you

[Benta]

Re1: for optocouplers there are a couple of tricks.
1.1: Broadcom (ex Avago) and others offer optocouplers with a defined creepage distance of >8 mm over the body of the part.
1.2: by milling a slot in the PCB between input and output, creepage is changed to clearance distance.

Re2: by doing that, you're no longer talking about creepage or clearance, but isolation thickness.

[TimNJ]

Thank you

Couple of more quesitons:

1) About the 8mm (point 4 above) is that also between two sides of a optocoupler where one side is mains and the other is isolated 3V3?
I cannot find an optocouplers with 8mm gap between the two sides and most of them are 4mm and they are rated at few kV. How does that work?

2) Also what are the rules and regulations for the same application if I want to place components with high voltage difference (275Vac)on top of each other on opposite sides of the PCB? For example:
- live trace on top and neutral trace on the bottom or
- either or the mains traces on top and 3V3 isolated on the bottom
Can I do that?

Thank you

1. Check Vishay TCLT101x series or Everlight EL101x series

https://www.vishay.com/docs/81256/tclt1010.pdf
https://www.everlight.com/file/ProductFile/201407061745083848.pdf

If you want to use through-hole, like LTV817 or similar, you can get an extended lead version, or if you use the standard version, put a slot in the board under the optocoupler. The clearance can be 6.5mm as long as the creepage is 8mm. (That's according to the medical standard. Industrial/telecom use is allowed to be lower, but just being on the safe side.)

2. It's no problem to put opposite polarity of mains on either side of the PCB. FR-4 can withstand several KV between top and bottom conductors without breakdown. BUT, you need to still be cognizant of creepage around the edge of the board. i.e. If you put a line trace on the edge of the PCB, and neutral trace on the bottom, also right on the edge, then the creepage is only the thickness of the PCB! So, back off your traces from the edges, if necessary.

To your second point about mains on one side and isolated on the other...how would you do that with an optocoupler? At some point there will be both mains and isolated on the same side. It's not typical to do it this way and I'm not optimistic it will work out as well as you hoped, especially if you have any through-holes or vias.

[ricko_uk]

Thank you Benta and Tim,

what is the required isolation thickness for 275Vac? Where can I find official guidelines/table?

What about in a 4 layer board? What is the maximum voltage between the top layer and the first plane? The isolation is a lot thinner (I think microns). Are there standards/tables for that?

With reference to the attached schematic, you would then recommend I stick to 8mm creepage (by cutting a slot) but can go to 4mm clearance? Is that correct or did I misread?

Tim, in reply to your point:

To your second point about mains on one side and isolated on the other...how would you do that with an optocoupler? At some point there will be both mains and isolated on the same side. It's not typical to do it this way and I'm not optimistic it will work out as well as you hoped, especially if you have any through-holes or vias.

That was just for general traces, not specifically for the optos.

Thank you

[TimNJ]

FR-4 has a dielectric strength of around 20KV/mm, so for a 1.6mm PCB, it can hold off 32KV without breakdown. 275V is nothing. 

The requirements for mains spacing and pri-sec spacing vary depending on the intended application of your circuit, board contamination level, altitude, and peak working voltage.

The simplest way to comply with just about every safety standard is 8mm creepage/8mm clearance. The minimum clearance per IEC60950/62368 (ITE/ICT) is 4mm. But, if you want to use in altitudes up to 5000m, which is a typical requirement, you need to to multiply the clearance by 1.48...so the requirement becomes 5.92mm. The creepage value must equal or exceed the clearance value (by definition), so the creepage requirement also becomes 5.92mm. If this was for medical equipment, again the requirements vary by intended usage, but in general the creepage always needs to be 8mm, and the clearance can be 6.45mm (2xMOPP) or 7.40mm (2xMOOP).

This is why I just suggest to use 8mm/8mm to cover all possible requirements worldwide. Assuming this is just a project for yourself, you can safely go with 6mm/6mm.

[coppice]

Re1: for optocouplers there are a couple of tricks.
1.1: Broadcom (ex Avago) and others offer optocouplers with a defined creepage distance of >8 mm over the body of the part.
1.2: by milling a slot in the PCB between input and output, creepage is changed to clearance distance.

Re2: by doing that, you're no longer talking about creepage or clearance, but isolation thickness.

The widened optocouplers do the job, but take so much space the slotting approach is preferred by most people. Slotting is a wonderfully simple way to get excellent isolation in a lot of situations. Unless you go crazy with slotting it doesn't seriously impact board strength, and its cheap.

[ricko_uk]

Thank you Tim and Coppice.

Tim, what about TO247 packages then? The mosfets used in the reference design (sch also attached) are TO247 and they would have the full voltage across their terminals which are only 3mm apart.

How does that work in that case? For those components?

Thank you

[Benta]

Re1: for optocouplers there are a couple of tricks.
1.1: Broadcom (ex Avago) and others offer optocouplers with a defined creepage distance of >8 mm over the body of the part.
1.2: by milling a slot in the PCB between input and output, creepage is changed to clearance distance.

Re2: by doing that, you're no longer talking about creepage or clearance, but isolation thickness.

The widened optocouplers do the job, but take so much space the slotting approach is preferred by most people. Slotting is a wonderfully simple way to get excellent isolation in a lot of situations. Unless you go crazy with slotting it doesn't seriously impact board strength, and its cheap.

You misunderstood my post. The Avago 'couplers I'm talking about are still 0.3" spacing, but have a modified DIP-8 profile to ensure 8 mm creep distance across the part. It's just an epoxy mold shape modification. The PCB slot is still needed.

[coppice]

Re1: for optocouplers there are a couple of tricks.
1.1: Broadcom (ex Avago) and others offer optocouplers with a defined creepage distance of >8 mm over the body of the part.
1.2: by milling a slot in the PCB between input and output, creepage is changed to clearance distance.

Re2: by doing that, you're no longer talking about creepage or clearance, but isolation thickness.

The widened optocouplers do the job, but take so much space the slotting approach is preferred by most people. Slotting is a wonderfully simple way to get excellent isolation in a lot of situations. Unless you go crazy with slotting it doesn't seriously impact board strength, and its cheap.

You misunderstood my post. The Avago 'couplers I'm talking about are still 0.3" spacing, but have a modified DIP-8 profile to ensure 8 mm creep distance across the part. It's just an epoxy mold shape modification. The PCB slot is still needed.

An optocoupler plastic body thick enough to have 8mm of surface between the pins has been commonplace for decades. I thought you were referring to the splayed legs versions, that put in the pins on the PCB far apart.

[TimNJ]

Thank you Tim and Coppice.

Tim, what about TO247 packages then? The mosfets used in the reference design (sch also attached) are TO247 and they would have the full voltage across their terminals which are only 3mm apart.

How does that work in that case? For those components?

Thank you

3mm is just about enough, in the absence of a fuse, or if placed before the fuse(s). Refer to my first post. On that note, I think you should really fuse the load circuit.

By the way, any reason you are not just using a TRIAC? If we use the "power loss per dollar/pound", MOSFET based SSR almost always has higher loss compared to a TRIAC. The issue is mainly that high voltage MOSFETs still have relatively high RDSON and you can't avoid the body diode drop.

Have you identified a particular need for using MOSFETs? Maybe you need exact control of the switch on/off time?

[ricko_uk]

Thank you all.

Tim, the only reason is that the guy I am doing this for specifically asked to copy his reference design. Not other reason. Apparently he made a prototype and he is happy with it, I am just making a proper PCB for him.

Thank you again for all feedback!