0
\$\begingroup\$

According to a UL/ULC standard, the spacings between traces of the PCB is specified as below table

enter image description here

I am quite curious about the spacings. Because there are many IC circuit components with very short clearance due to the trend of smaller IC. Such as the MCU chip the clearance between pads is as small as 0.3mm. enter image description here

quote from the ULCS531 standard

My device is a 24VDC powered smoke detector that has a PCB inside. enter image description here

\$\endgroup\$
8
  • \$\begingroup\$ 0.3mm is normal. Below that I become unsure if a special fab is needed or not. \$\endgroup\$
    – DKNguyen
    Jan 21, 2020 at 3:28
  • \$\begingroup\$ @DKNguyen According to the standard note e, the minimum spacings between traces is 0.8mm. Obviously this is a large clearance that's to say my PCB traces spacings can not meet the requirements? Am I right? \$\endgroup\$
    – lukeluck
    Jan 21, 2020 at 4:05
  • \$\begingroup\$ I don't know about that. But I can tell you that the spacing between pads on a MASSIVE 1.27mm pitch SOIC is still 0.6mm between pads and there are many ICs with far smaller pin pitches. \$\endgroup\$
    – DKNguyen
    Jan 21, 2020 at 4:16
  • 1
    \$\begingroup\$ ULC S531 is apparently a specification for smoke alarms. If you aren't designing a smoke alarm, it has nothing to do with your project. \$\endgroup\$
    – The Photon
    Jan 21, 2020 at 5:03
  • 1
    \$\begingroup\$ Assuming you are NOT designing a smoke detector, please refer to IPC2221A and/or UL60950-1 for general guidance on creepage and clearance distances for PCB design. \$\endgroup\$
    – user57037
    Jan 21, 2020 at 5:29

2 Answers 2

1
\$\begingroup\$

The standard you found is apparently a specification for smoke detectors, and even more specifically for ones to be marketed in Canada. If you aren't designing a smoke detector, or aren't in Canada, don't worry about that standard.

UL specifications mainly relate to electric shock and fire safety. There are different ones for different kinds of products, like for consumer electronics, for IT equipment, etc. The one I know best is UL 61010, which applies to "Electrical Equipment for Measurement, Control, and Laboratory Use". But the specs I've looked at for IT and consumer electronics aren't much different.

In these specs, the specified clearance distances apply between potentially hazardous voltages and conductors that connect to potentially user-accessible locations. There's no need (for safety reasons) to isolate between one hazardous voltage and another, and there's no need isolate between conductors carrying non-hazardous voltages.

This generally means you divide up your design into a "potentially hazardous" region and a "potentially user-accessible" region, draw a line between them, and make sure that one side is isolated from the other by respecting the required creepage and clearance distances between conductors on one side and the other.

Potentially hazardous voltages are typically defined to be voltages over 48 V. If your design doesn't produce a voltage over 48 V anywhere, you will have essentially no requirement isolation for protection from electric shock. (But consult a safety expert familiar with your application area to be sure you're following the correct specifications for your project)

If you're designing a medical device, or one like a smoke alarm that's related to life safety, you will probably need to meet more stringent requirements. In that case, you should be talking to the PEs on your team rather than random people on the Internet.

So, if you aren't designing equipment related to life safety, and 24 V is the highest voltage present in your system, your copper trace and space limitations probably don't depend on any UL spec, but on the manufacturing capabilities of your PCB manufacturer.

Typical minimum spacing for very low cost designs is 0.008" or 0.2 mm. Spacing down to 0.004" or 0.1 mm is very widely available without paying very much cost premium. Spacing down to 0.003" or 0.075 mm is widely available (For finished copper thickness not greater than 36 um) at increased cost. For anything smaller than 0.075 mm, consult your manufacturer before proceeding.

\$\endgroup\$
5
  • 1
    \$\begingroup\$ My product is a 24VDC powered smoke detector. \$\endgroup\$
    – lukeluck
    Jan 21, 2020 at 5:48
  • \$\begingroup\$ @lukeluck, and are you going to use it in Canada? \$\endgroup\$
    – The Photon
    Jan 21, 2020 at 5:48
  • \$\begingroup\$ yes,@The Photon the device will be sell in Canada. \$\endgroup\$
    – lukeluck
    Jan 21, 2020 at 5:55
  • \$\begingroup\$ Then you need to get a Canadian licensed engineer on your team who knows about fire safety equipment and ask them instead of people on the Internet. \$\endgroup\$
    – The Photon
    Jan 21, 2020 at 5:59
  • 2
    \$\begingroup\$ As I noted in my previous comment, the document you posted references another document that you need to dig up: Evaluation of Reduced Spacings on Printed-wire boards. You need to find that document because if your PCB complies with it, then that is a valid exception to ULCS531. Take note of the 12.5mA exception also. If your circuit consumes very little power then you can just put a 2.2k resistor externally in series between your 24V supply and your PCB, then the whole PCB will be exempt from the clearance specification. \$\endgroup\$
    – user57037
    Jan 22, 2020 at 0:43
0
\$\begingroup\$

Generally the PCB manufacturer will announce their capabilities.

capabilities

The specs that you shared is not from manufacturability angle but rather from certification point of view. If you notice, they are different for different voltage ratings. These specs take into consideration PCB surface contamination and possible arcing situations which can shorten the life of your product.

\$\endgroup\$
3
  • \$\begingroup\$ My device is 24VDC powered .so according to the standard, the minimum spacing between traces is 0.8mm. Obviously 0.8mm is a so large clearance that my PCB can not satisfy. Is my understanding right? \$\endgroup\$
    – lukeluck
    Jan 21, 2020 at 3:58
  • \$\begingroup\$ Are you sure your specs are trace spacings? These spacings will make a lot of products to fail the certification. Even so, your MCU will be working on 3.3 V for which the trace spacings will be lower. Check this - smps.us/pcbtracespacing.html \$\endgroup\$ Jan 21, 2020 at 4:05
  • \$\begingroup\$ I already checked the same web calculator but still , find no answer to my confusion. Can you help clarify the quoted standard I updated \$\endgroup\$
    – lukeluck
    Jan 21, 2020 at 4:13

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.