Inner layer track distances

[sh-eda]

Hi

I am working on a PCB which is going to work at 240Vac mains. I am struggling with creepage and clearance distances, so
the only answer I can see is to put the mains Live and neutral on inner layers.
I have looked at the spec and see that the clearances for an inner layer will be >0.25mm. Can I check that this is true? I assume this applies between layers as well? The board I working on will be 2.4mm thick.
I realised the tracks will need to be thicker on an inner layer because of poorer heat dissipation.

Thanks

 

[FvM]

To which spec are you referring? I noticed that different specs have different assumption about the lateral (horizontal) and vertical voltage strength of inner layer insulation, resulting in different spacing rules. Apparently some specs assume that the layers may be delaminated, cancelling the effective trace encapsulation at inner layers. Similarly the uniformity of prepregs might be doubted.

 

[sh-eda]

Hi
Interesting.
I should say standard. This is really what I want to check.
I am looking at the IPC-2221A electrical clearance table, though not the latest copy. I have been searching the internet and I see 0.25mm as a common figure. I am not intending to have Live, earth and Neutral cross anywhere on the board.

 

[FvM]

The IPC-2221A rules are only clear at first sight, I fear. For mains voltage you should also consider overvoltage categories and easily end up in the > 500 V category with tenfold clearance.

I doubt that IPC-2221A actually addresses this kind of voltage stress otherwise it would refer to respective technical standards about isolation coordination.

 

[sh-eda]

Beyond 500V peak it uses a simple formula for inner layers.
0.25mm + 0.0025mm/Volt x (voltage above 500V)

So for 1KV the inner layer distance would be
0.25mm +0.0025mm/v x 500v = 1.5mm

What other standards have you seen? or I could refer to?

 

[FvM]

e.g. IEC-1010/EN61010 and ECMA-287

 

[marce]

You are correct inner layer spacing is only 0.25mm up to 500V, IPC-2221A is one source another is a UL spec (I am not at my machine so cannot get the specific number).
The specs such as 60590 61010 specify creepage and clearance THROUGH AIR, inner layers of a PCB are an embedded in an insulator so these spacing do not apply. In over 30 years of playing around with PCBs this is the most frustrating problem I face, with people coming up with all sorts of myths for inner layer clearance, half the distance on the outer layers being a favourite...
Nope its 0.25mm
I will try and dig out the UL spec where it states quite clearly that this does not apply to inner layers...
You can also ditch the spacing's on outer layers (through air) if you have your boards conformally coated.

 

[Mattylad]

What Marc says....

Don't forget that when you use inner layers you will need to derate your tracks as they cannot dissipate heat as well.

Still makes mains voltage layout much easier though, not to forget that the pins on the outside still need full clearance from each other.

 

[marce]

Looking further into this, the issue is further complicated by EN 61010-1 3rd addition, which has rewritten the requirements for inner layers... This as far as I can tell is not reflected in 60950, so when I can get all the relevant up to date specs I will re-evaluate all the requirements and whether they apply to the world in general or whether different regions are at different levels.
De-rating for inner layers is so olde worlde Matt, embrace IPC-2152 for current carrying capacity, the old stuff was so out-dated and based on some very primitive testing....
Another calc for current based on IPC-2152:
https://www.smps.us/pcb-calculator.html

When I have done some further research into the specs I will report back.
At the moment based on section 6.7.2.2.3 of 61010 the inner spacing has increased to 0.4mm <150V 1.5mm > 150. I do need to confirm these figures... Interestingly IC isolators such as Adum devices do break the 60101 rules but are compliant to another standard that involves actual testing and so can be used on 61010 compliant equipment...
This mess of different specs etc. is a pain is your equipment to 61010, 60950 or some other spec.

 

[sh-eda]

Ok Thanks for the all your efforts I really appreciate it.

I will see if I can get EN 61010-1. I am looking at ECMA-287 as well which was mentioned before
As you say, this is not very clear at all.

Looking at the PCB the maximum inner clearance between Live and earth tracks etc, I will be able to achieved is about 1.8mm.

Yes I am planning to make the track width much larger than I would have been able to on the outer layers.
I have not seen the https://www.smps.us/pcb-calculator.html website so thanks for that. I've been using a different one, so I will have a look.

 

[marce]

Edition 3 is the critical one...
As said I do not know whether this has been globally accepted, I do now it is relevant in Europe.

Also have a look at the Saturn PCB toolkit....
Heat dissipation can be influenced by many things, especially multi-layer designs with copper planes. My preference for high current (anything over 5 amps) is to have a copper pour so I have the maximum amount of copper in the available space. I will also try and duplicate the pour/tracks on other layers if I have the room.

 

[ArticCynda]

A clearance of 0.25 mm is really too small for 230 V AC, you never know what might happen in case of an insulation breakdown caused by excessive force on the board for example. I keep a clearance of 1 mm in mind as a rule of thumb, regardless of the layer, for every tracks carrying 100 V DC or more.

 

[sh-eda]

I've managed to see IEC61010-1 3rd edition.
Sections 6.7.2.2.3. There's also table K1.3.3 (Inner insulation layers of printed wiring boards)
Yes I can see that 0.4mm is the minimum distance between two adjacent conductors.
However, there's a note a these values are independent of the overvoltage category?
So this does not take in account surges? The pcb that I am working on will always be fitted with main filters (such as IHF50). but I am assuming I will have to fit main surge arresters?

 

[marce]

Again we get into an area of ambiguity, from my experience of doing numerous boards with mains voltages (8 years doing Gen Set controllers) we always worked on the peak mains voltage, over voltage and spikes were not taken into account. That said there usually has to be some form of protection, MOV or similar. If you start taking into account spikes and overvoltage you will find that the layout becomes impossible....
I believe I have a copy of K1.3.3 in a app note regarding isolators that in theory break the rules set down in 61010. As I said there is a problem here as some equipment is built in reference to 60950 (Information Technology Equipment) and some to 61010 and some to just general rules of thumb. Like a lot of committee based standards, they are confusing and there seams to be no harmony between the various standards, and like IPC standards if you study them carefully you will find often conflicting information between standards that cover the same aspects of design. The trouble is trawling through all this information is time consuming and tedious, but when I do get updated copies of all the standards I will again (for the hundredth time) trawl through them. An interesting point is that much equipment on sale today actually breaks this standard having been designed to the old standard.
I do fight against the complexity of PCB related standards, one in particular is now getting very silly and overblown, IPC-7351 for mainly in my view commercial reasons, I will be publishing my tirade against the unnecessary complexity that is taking over this standard in the near future....
Standards should be easy to follow and made as simple as possible regarding the subject covered, the problem is they are controlled by committees and all tend to get over bloated, unfathomable and complex.

 

[sh-eda]

Yes I agree with what you say, I wish it was clearer. I'm wading through the standards and it's not straight forward. They don't appear to be written by people who use them.

I'm undecided what to do at the moment, I think the distance I can achieve would be ok (1,8mm, maybe more). If I fit surge arresters. We also do fit fairly heavy duty mains filters. Unfortunately the application is industrial and safety related, so it's possible that the mains quality could be poor. That's why I'm being careful.
At the moment I'm trying to work out what sort of surge protection (MOV) to fit and which configuration.

Thanks