8
\$\begingroup\$

I am designing a PCB for use with an Arduino mega and I am wondering if there is a good rule for how much space I should leave between the edge of the PCB and various items like:

  • traces (ground, 5v supply, 9v supply, and 5v digital signals)
  • surface mounts
  • small through holes (capacitors)
  • mounting holes (for screws)
  • large through holes (power supplies)

I currently have 0.1" around everything except of a through hole for a DC jack, which comes .05" from the edge. Can I remove some of this space and not hurt my design?

\$\endgroup\$
  • 1
    \$\begingroup\$ Are you working with a specific fab house, or wondering if there's a generic "maximum minimum" that is safe no matter which Chinese fab is making your design? \$\endgroup\$ – ThreePhaseEel Sep 10 '15 at 4:17
  • \$\begingroup\$ I'm using expresspcb.com \$\endgroup\$ – Hoytman Sep 10 '15 at 15:59
  • \$\begingroup\$ Then ask expresspcb.com. How is this not obvious? \$\endgroup\$ – Olin Lathrop Sep 10 '15 at 16:19
  • 7
    \$\begingroup\$ Because this is my first PCB. \$\endgroup\$ – Hoytman Sep 11 '15 at 18:59
8
\$\begingroup\$

traces (ground, 5v supply, 9v supply, and 5v digital signals)
surface mounts
small through holes (capacitors)

Collectively, all these are covered by the minimum copper to board edge clearance parameter.

enter image description here

The value is driven by the precision with which the PCB fab can register the board before it's routed. Typical value is 0.020". Narrower clearance is possible, but the fab may charge extra for additional precision. So, check with the fab, the clearance should be on their "capabilities" page (like this one).

mounting holes (for screws)

Distance of mounting holes for screws is driven by a mechanical considerations. My rule of thumb is to keep the distance between the edge of the hole and edge of the board at least as big as the diameter of the hole. But this can vary greatly depending on how much vibration your assembly will see, and how heavy are the components on the board.
[hint: Separate question.]

\$\endgroup\$
  • 2
    \$\begingroup\$ Worth noting that for the Wun Hung Lo board house, 0.030" is probably safer. \$\endgroup\$ – Matt Young Sep 10 '15 at 4:23
  • \$\begingroup\$ The minimum clearances and other parameters are usually specified in a DRC (Design Rule Check) file, and used to verify the layout meets these rules before Gerbers are generated. \$\endgroup\$ – tcrosley Sep 10 '15 at 5:02
  • 1
    \$\begingroup\$ The PCB layout software usually has some default value for each kind of clearance. The actual value for the clearance, though, should come from the PCB fab side of things. \$\endgroup\$ – Nick Alexeev Sep 10 '15 at 5:06
  • \$\begingroup\$ I generally plan for 25mil, though for high-quality board houses I have gone down to 15mil. That's pushing my limits though \$\endgroup\$ – DerStrom8 Sep 10 '15 at 16:25
4
\$\begingroup\$

In your case (and this is true for all but the cheapest Wun Hung Lo fabs, from what I can tell), you are safe with a 20mil clearance, as per the ExpressPCB design rules doc.

\$\endgroup\$

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.