I am currently designing a PCB for a project including PID-control of a heater. The heater runs on mains (220V) and is controlled using zero-crossing switching to regulate the power and minimize EMI and THD. I already designed multiple PCBs , also ones with mains, but never low and high voltages on the same board. By nowenter image description here I have e prototype-design, where I made the following safety considerations:

  • strict separation (HV,leftside - LV, right side, see line on top silk layer)
  • connection HV-LV only via optotransistor/-triac (U1 and U2) and a switching converter U6 including a isolation transformer
  • further protection with MOV(R6), fuse (F1) and use of a snubberless triac Q1
  • copper planes of LV part start only after the last everything is converted to LV

Since I do not really have any space constraints I designed everythig with a lot of clearence (grid is 1mm) and used 2mm traces for the AC-powerlines. The PCB is then mounted in a metal box connected to PE or in one out of isolation material. My main concern is that there are three JST plugs on the LV side (U4,7,8) that connect to rotary encoders, screens,etc, that are accessible to the user. While I am confident about the isolation on the PCB I still wanted to get second takes on the design, especially regarding the connections to the user-accesible features. Are there additional considerations to make in this case?

Any feedback regarding any part of the design is appreciated!

  • 1
    \$\begingroup\$ What devices are U1, U2 and U6? I would consider treating N to earth with the same respect as you treat L to earth. \$\endgroup\$
    – Andy aka
    Commented May 25, 2020 at 16:18
  • \$\begingroup\$ Is the placement and terminal layout of P1 and P2 fixed? Or can you move them a little bit, and could you swap L and N on one? \$\endgroup\$
    – marcelm
    Commented May 25, 2020 at 18:14
  • \$\begingroup\$ No P1 and P2 are not fixed, would you place them further apart? Yes you could swap it on one (I assum you would do it for shorter traces) but the L of P1 still needs to go through the fuse. \$\endgroup\$
    – Beorn
    Commented May 25, 2020 at 19:12

2 Answers 2


I have the following feedback on your layout, roughly ranked by importance:

  • Your PE trace is far too thin. In the case of a live-earth short downstream of your board, you run the risk of vaporizing this trace before the fuse or a breaker / GFCI trips. You want mains traces as short and as fat as possible; of these PE is the most important for safety.
  • You could increase the clearance between the different mains traces. HV - LV isolation is top priority, but L-PE and N-PE are also important, and if you can manage, L-N clearance is also good. I would aim for at least 4mm clearance wherever feasible. I realize that's not possible everywhere, but there is room for improvement.
  • Consider making a slot in the PCB below U1 and U2, between the HV and the LV side. This further increases the creepage between HV and LV.
  • Keep mains traces as short and fat as possible; to keep resistance low. In case of a fault, you want a low resistance so a breaker/fuse trips decisively. Use top and bottom traces if appropriate. Your L trace is a bit too long for my taste. Keeping traces short also helps with EMI. I would prioritize keeping the traces "on the power path" (between P1, P2, F1, Q1, R6) over those "on the signal path" (dealing with R1, R4, R5, U1, U2).
  • Clearance between the pins of Q1 is particularly low. I like using a footprint with the pads further apart, and spreading the triac's legs out before soldering. See e.g. this answer.
  • Are you using huge footprints for R1 and R5 for clearance and power dissipation? You can also use several smaller resistors in series to achieve that. Use similar value resistors, assume voltage distributes equally over them so you can add their voltage ratings, and derate generously. Like a factor 3 or so.
  • \$\begingroup\$ Hi marcelm, thanks for your feedback! I am definetly going to revisit the pcb with your comments in mind. Especially the clearence of the TO220 package, it seemed also to me very small to beign with... R1 and R5 are for current limiting and take about 0.57W continuous each (27kOhms each) and I have them rated for 2W. I thought this would be sufficient. Also I did not want them too small so I still can solder them easily. \$\endgroup\$
    – Beorn
    Commented May 25, 2020 at 19:10

I've printed PCB's with HV/LV split and mostly avoided the issue by far exceeding the requirements for clearance/creepage and used an isolation transformer. I'm sure you've already looked up the distances but here's a reference:


Also if you're worried about spikes blowing your equipment and getting back to the user, you could add an inline fuse where the HV comes in and then a thyristor to ground directly after to shunt the fuse to ground if there's a spike. It will blow the fuse to isolate the circuit.

  • \$\begingroup\$ Hi Kent, thanks or your feedback! To catch voltage spikes I already placed a varistor at the input and there is an inline fuse (f1) but it is also for the load, so probably about 10A-16A. I am not quite sure how your fuse-thyristor combination looks though but I wopuld be happy to hear some elaboration! \$\endgroup\$
    – Beorn
    Commented May 25, 2020 at 19:20

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.