4
\$\begingroup\$

A general question regarding PCB design of equipment to the 60070-11 standard for intrinsic safety type "ib" or better. Often, and more so than ever, ATEX certified electronic equipment requires complex electronics and multilayer, high density PCB design.

The equipment I am currently developing is being designed from the start with it being equally ATEX certified (and eventually IECEx), besides it having the CE and or FCC certification. So on the current PCB design the over voltage Zener protection is included with the correct power ratings, the infallible resistors in series with large inductances, fuses etc. all allowed for from the start. This prevents us from having to re-route the board for an ATEX specific product. For non ATEX the protection components are in most cases left out or replaced by 0 ohm shunts etc.

One issue I'm having with the PCB design to 60079-11 is what appears to be a rather limiting minimum separation distance for the Overvoltage Category, which in our case is 10V, Category I as it is all 3,3V digital and some analogue. One 12V booster charge pump for the OLED display, but this is low current and fused at < 150mA.

In Annex F, "Alternative separation distances for assembled printed circuit boards and separation of components" table F1 - Clearances etc. outlines this, and one can see the lower limit is basically 0,2mm for most cases, including encapsulation, coating etc.

It seems this lower limit is "out of touch" with modern PCB designs that use 0,5mm and even 0,3mm pitch BGAs, or > 10 layer stackups for the PCBs. In my case, I do have a 0,5mm pitch BGA and an 8-layer 1,6mm PCB. To route the BGA lines I am obligated to have conductor separation to < 0,2mm (0,17mm or so), and in another case, a small analog BGA with 0,3mm pitch, this separation is even lower actually 0,1mm on two or three pins.

The other issue is the layer to layer separation which does not appear to be treated in any way by this standard (other than minimum conductor separation as in table F1). The PCB manufacturers build up the stack-ups with prepregs often less than 0,2mm thick and in most cases even less than 0,1mm. Cores can be 0,2mm readily available... but this again creates a situation with conductor to conductor separation to < 0,2mm minimum as in table F1.

So what gives than ? According to 60079-11 most of these PCBs stacks and BGAs etc. would practically be uncertifiable since the 0,2mm lower limit on conductor separation is clearly unachievable ? Is there a work around that I may have missed in the standard ?

I have seen ATEX certified mobile phones being commercialized, which implies they most likely contain BGA components and multilayers (> 8 layer), high-density PCBs. How do they get Intrinsically Safe certification for Zones 1 and 2 which still require 60079-11 ??

Is pure testing in an ATEX certification laboratory the only way to ensure a pass for intrinsically safe certification in this case ??

thanks in advance for any suggestion or references that may treat this in the 60079-11.

Mike

\$\endgroup\$
  • \$\begingroup\$ From what I recall, one way is to mould in the whole PCB with some substance that lead heat, then treat it as a black box. On the supply, you toss on a fuse, several zener diodes and a current limiting resistor. This way you don't need to care where on the PCB that a short circuit occurs. The only thing that's important is that the product does not generate a lot of heat in a limited area upon failure. Getting rid of "pyrotechnical" components like tantalum and electrolyte caps might also be a good idea. \$\endgroup\$ – Lundin May 29 '18 at 13:18
  • \$\begingroup\$ Hi, yes, encapsulation by conformal coating is an option, but those in the know charge alot for mass production with conformal coating. It ends up that zeners, fuses and resistors are cheaper overall. Then there is also the issue with heat dissipation ... Tantalums and electrolytics are not a good idea in this case, and besides ceramics have better specifications and not problems with polarity etc. \$\endgroup\$ – citizen Jun 25 '18 at 7:28
  • \$\begingroup\$ You have to use both methods, depending on EX zone. A metal film resistor is considered safe as it will burn off clean, but when it does, the heat must spread across a larger area. This is best solved with some coating/moulding that lead heat. Indeed it is not cheap - nothing EX is cheap. \$\endgroup\$ – Lundin Jun 25 '18 at 7:33
  • \$\begingroup\$ Hi, I am hoping not to have to use the conformal coating. The resistors should be selected from calculations in IEC 60079-11 to ensure they can dissipate the required heat without the need for them to "burn off clean". If anything its the fuses that may go up in a "puff of smoke" and these are generally encapsulated in a disipative ceramic and capped to some level of protection. There are fuses around that are recommend for intrinsic safety... \$\endgroup\$ – citizen Jun 26 '18 at 8:02
  • \$\begingroup\$ Now that you mention it, I remember using 2512 1 Ohm or something similar for the resistors. MK2 through-hole should work too. \$\endgroup\$ – Lundin Jun 26 '18 at 9:56
4
\$\begingroup\$

What is important to realize is that the distances are necessary only if the intrinsic safety will be compromised by a short circuit (that is the failure model, if you don't have the distance you must assume a short circuit between the lines).

As you design your device your concept should be aware of that and your ICs should be in an area where the intrinsic safety will be held up even if a short circuit occurs. That way there is no distance requirement anymore and you can use BGAs and other fine pitched devices.

The same holds true for the PCB stack. In critical areas you have to have those distances but in protected areas you can get as close as you want. Layer to layer separation falls under "Separation distance through solid insulation", so no special rule is applied there.

I'm not an authority in the field and can give you only the recommendation to involve your certification inspector early in the process and talk through your concept before doing major work on it. We had some serious changes in our circuits because of our concept not matching what was expected and misunderstandings of the standard.

\$\endgroup\$
  • \$\begingroup\$ Hi, yes that makes sense. The circuit is protected by an IP68 product case and the electrical protective components, fuses, zeners, resistors and other voltage/current limiting devices and "the intrinsic safety will be held up even if a short circuit occurs" as you suggest. The device may stop working becuase of a blown fuse, but this is built in and maintenance can be performed if required. \$\endgroup\$ – citizen May 24 '18 at 12:46
  • \$\begingroup\$ In this case the product may include a small value but large case disipative resistor creating a low imdeance path to ground or a semi-short-circuit, but as long as it does not exceed certain temperatures limits or high currents through inductors, it would still be intrinsically safe nevertheless, regardless of it draining the battery in 20 minutes etc. instead of 5 hours lol ... I guess though I won't be doing that ;-) \$\endgroup\$ – citizen May 24 '18 at 12:51
  • 1
    \$\begingroup\$ @citizen Well usually you will find some places where you need to get the distance requirement. Places like connectors and the battery terminals are always critical (limit the energy which can get out of your device via that connector). I cannot stress enough how important it is to contact the certification body early. \$\endgroup\$ – Arsenal May 24 '18 at 13:02

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.