Notching high voltage PCBs

Discussion in 'General Electronics Chat' started by Skeebopstop, May 13, 2009.

  1. Skeebopstop

    Thread Starter Active Member

    Jan 9, 2009
    358
    3
    Hi All,

    Recently I have noticed a design where they notched some high voltage tracks. I am reasonably new to high voltage so perhaps there are things like creapage clearances I am overlooking.

    The query is however, that I looked into IPC2221 and found that the clearance presented on the coated PCB should have been sufficient for the 400V, but yet they notched it anyways?

    Any input into some reasoning behind their notching would be much obliged.

    Regards,

    James
     
  2. aliensong

    New Member

    May 13, 2009
    7
    0
    Hi, James

    When it comes to high tension electricity, you'd better to call a electrician to deal with. At the same time, you can say your question to electrician for help! ;)
     
  3. Darren Holdstock

    Active Member

    Feb 10, 2009
    262
    11
    I can't quite picture it - do you mean a chunk of track has been bitten out to give obvious extra clearance for an adjacent bit of copper, or are the tracks in question notched in a puzzling way?
     
  4. DonQ

    Active Member

    May 6, 2009
    320
    11
    Pictures! We need pictures.
     
  5. THE_RB

    AAC Fanatic!

    Feb 11, 2008
    5,435
    1,305
    It's pretty common on PCBs here in Australia where the mains is 240vac. The routed holes in the PCB have less chance of an arc jumping across the airgap than tracking across the surface of a PCB. Another problem is that a PCB will attract some dust which is hydroscopic (absorbs water) and can over time make a film on the PCB which is much more likely to arc across than a 4mm air gap cut into the PCB.
     
  6. Skeebopstop

    Thread Starter Active Member

    Jan 9, 2009
    358
    3
    I am in Australia too. Here is an image of it where I measured the 'minimum' clearance. Yes these are uncouted exposed leads, but according to IPC2221, at < 3000m elevation 1.8mm is enough for up to 500V.

    We will never exceed 450V.

    So I ask myself, why bother? I realize there is no real harm in doing so but is more a question of, what if I 'forget' to do this during design.

    Thanks
     
    • PCB.JPG
      PCB.JPG
      File size:
      143.8 KB
      Views:
      76
  7. Darren Holdstock

    Active Member

    Feb 10, 2009
    262
    11
    Oh right, a milled slot separating tracks. Or in this case, 133 little drill holes in a row. It's just standard practice to increase creepage distances, though the clearance distances will remain the same. If this is beyond what the spec requires, then maybe the designer is playing it safe. Conformal coating can be badly applied, and PCBs can be covered with moisture and dirt, but a slot in board is a fairly reliable way of maintaining electrical separation.

    What are the creepage and clearance requirements of IPC2221, just out of interest?
     
  8. THE_RB

    AAC Fanatic!

    Feb 11, 2008
    5,435
    1,305
    Ouch! 2mm gap between 450v and a ground plane??? :eek:

    The IPC spec might be fine for zero humidity air in a laboratory when the PCB is new and NOTHING has contaminated your PCB, but seriously you might want to look at some commercial PCBs that have mains rated tracks. I was a TV repairer for a lot of years and some of the nasty things I saw arced across mains voltage tracks, and i've also seen lots of pro designed PCBs with very large clearances (these people know their stuff). Just look on a TV or monitor PCB at the mains voltage tracks, they will use 8-10mm from mains to mains or mains to gnd, AND if they are a quality manufacturer there will often be big slotted gaps of 4mm or 5mm rout between mains and gnd and almost definitely from mains to any user gnds which might be as much as 20mm gap.

    I'm kinda :eek: that you would put a 2mm gap from 450v to gnd... It's only gonna take one little roach with his front leg on track1 and his goopy arse dragging on track2... He'll explode, it will throw a solid ionised arc across 2mm through his bug-guts steam and your product is toast.
     
  9. Skeebopstop

    Thread Starter Active Member

    Jan 9, 2009
    358
    3
    Well the bug scenario would be unfortunate but in a design such as this, such clearances cannot be afforded. Televisions are big and bulky and have far more room than servo drives.

    Regardless, the design has been in the field for months now all around the world without an such incidence at up to 440V DC on the lines.

    I suppose from your response, the 'notch' can't hurt and if it is at all possible may as well throw it in. Let us suppose a very stringent design however, where the notch could not be placed due to space requirements. Yes there are potential concerns for the lifetime of the product, but assuming decent conditions, IPC 2221 should be sufficient and as such 1.5mm is the rated bare minimum for exposed leads up to 500V.

    I see no reason not to trust IPC 2221 if push comes to shove and the design calls for extremely tight scenarios, naturally keeping in mind that the closer one gets to the minimum, probably the more the product will come back for service and becomes a costing debate.
     
  10. Skeebopstop

    Thread Starter Active Member

    Jan 9, 2009
    358
    3
    IPC 2221 doesn't mention anything about creapage. What is the best standard for creapage in PCB design?
     
  11. Darren Holdstock

    Active Member

    Feb 10, 2009
    262
    11
    There's a distinction between creepage and clearance. To be safe, always follow the definitions in the relevant standard, but they can be roughly defined as follows: Creepage is the shortest distance between two conductors, following the contours of the solid insulating terrain. Clearance is the shortest distance in a straight line between two conductive points when the insulator is an air gap.

    Clearance distances are shorter than creepage distances, so one way of meeting the creepage spec is to introduce a cutout in the PCB. Now the line of creepage to be measured has to go around the edge of the slot, greatly increasing the creepage distance. The adjacent conductors still have to meet the clearance spec, but this distance is much smaller.

    Another way of increasing creepage distance is to undulate the surface of the insulator, a good example being the ceramic insulators used on high voltage power lines.

    Take all voltages as peak, not rms, unless the relevant standard specifies otherwise. It gets more complex, taking into account the nature of the insulator, the operating environment, use of conformal coating, and degree of dirt contamination - a good overview can be found here.
     
  12. Skeebopstop

    Thread Starter Active Member

    Jan 9, 2009
    358
    3
    Thanks mate!
     
  13. Wendy

    Moderator

    Mar 24, 2008
    20,766
    2,536
    I remember working for Collins Radio on some old style telephone circuits. The traces were really long, and the voltage wasn't that high, but we would still develop shorts between traces. Never did see anything, but running a sharp tool between the offending traces cured a lot of them. My personal theory is they were growing dentrites (did I mention this was very old electronics?).
     
Loading...