Will I have any trouble routing the traces in this way? (VCC and GND)

Picture showing how the traces are routed through pads

Is it OK considering that the entire circuit current is under 50mA?

  • 34
    \$\begingroup\$ By the naming convention those look like connectors of some sort. If so, and if the pin order is not pre-determined, I would recommend putting Vcc in the middle and ground and data on either side so incorrect insertion does not reverse the power to whatever it connects to. \$\endgroup\$
    – Trevor_G
    Mar 28, 2018 at 16:23
  • \$\begingroup\$ Thanks for the tip, I never thought about it. Those are connectors for sensors like dht21 and such that dont come with a proper connector, only bare wires \$\endgroup\$ Mar 28, 2018 at 18:19
  • 3
    \$\begingroup\$ For sheer function, it should be no problem. If you struggle with passing EMC, this may or may not turn out to be a problem for high speed signals. Never encountered it myself, just been told about the phenomenon in an EMC class. \$\endgroup\$
    – winny
    Mar 28, 2018 at 19:14
  • \$\begingroup\$ Saw this on the hot network question list and misread it as "traceroute through a pad" and was wondering how that would work... \$\endgroup\$
    – Michael
    Mar 28, 2018 at 21:09
  • 2
    \$\begingroup\$ I would only warn about mechanical stress, connectors are among the first things to be torn out by mistake. Should it happen then it could brake the trace and make the hole circuit fail. So if you have the oportunity i would not make it go through the pad if you have free space. \$\endgroup\$
    – ndelucca
    Mar 29, 2018 at 12:29

6 Answers 6


There is no problem routing traces through pads (like you have done). Be aware when routing power/GND of the current that will be travelling through these traces. This will dictate trace thickness. In addition, search for "power planes", "ground pours" for more information.

I can see where your confusion may come from. I'm not a fan of how Eagle renders traces connecting or passing through vias/pads.

When you do this:


This is how the copper will actually look on your PCB:


The thickness of the annular ring needs to be considered to ensure that it can carry the required current.


  • 11
    \$\begingroup\$ Good point about the current capacity. If something is soldered into the hole then there will be a lot more cross section available. But then what if it doesn't get populated ? \$\endgroup\$
    – Criggie
    Mar 29, 2018 at 1:01
  • 16
    \$\begingroup\$ Very nice graphics! \$\endgroup\$
    – clabacchio
    Mar 29, 2018 at 8:01
  • \$\begingroup\$ What did you use to make those graphics? \$\endgroup\$
    – user545424
    Mar 29, 2018 at 20:52
  • 1
    \$\begingroup\$ @user545424 OneNote with a stylus. Nothing fancy! \$\endgroup\$
    – Daniel
    Mar 29, 2018 at 20:56

No, it is not a problem routing through a pad. You might wish to consider adding ground and power planes to the design.


This should not be a problem if the pad is used, i.e. soldered before use. That will increase the current carrying capacity many times. Additionally, each side of the ring looks about as thick as the trace, so even without soldering, current capacity has been doubled.

But what does current carrying capacity really mean anyway? The pad is tiny, there will hardly be any voltage drop across it. And because it has greater surface area compared to volume, it will heat up less than the track. So unless there are a bunch of pads on the track, there is no cause to worry.

The real problem of course is if the pad is small, drilled and not soldered. In this case a track might be broken due to a bad drill bit. And, may not be noticed in a complex layout.

Much more importantly, an undersized pad may not be mechanically strong, especially when connectors are involved. I would widen the tracks on both sides of the pad just for the mechanical strength alone. Has saved me many times. The epoxy that holds the copper to the board can only take so much. Also make sure the drill holes fit tight.

  • \$\begingroup\$ the trace width is 24mils. Do you think i should thicken it even further? if yes, only in the area near the pad? \$\endgroup\$ Mar 28, 2018 at 19:12
  • 1
    \$\begingroup\$ Trace thickness is determined by the current and heat dissipation the trace needs to handle, and indirectly by whether the traces are on the top or bottom, or buried. 24 mils is gigantic for typical digital signals, but you'll need to figure your Vcc/GND current to determine adequate trace width. \$\endgroup\$
    – Bort
    Mar 28, 2018 at 20:15
  • 2
    \$\begingroup\$ If the connector will be subjected to repeated stress (frequent insertions, bent wires in enclosure etc.) I would thicken the track only near the connector pad, maybe about 5mm either side. It's fine as long as it does not violate clearance. Less of an issue in plated holes with pads on both sides, but why risk it? I'd think 0.8mm as safe (~32mil). Of course, even 0.1mm trace would be overkill for humidity sensor current, but that's not the issue here. \$\endgroup\$
    – Indraneel
    Mar 28, 2018 at 20:38

If the connections to those pins are the same VCC and same ground you will have no issues.

Physically the copper track will only go as far as the pad it wont actually be left hanging over the hole upon manufacture.


In relation to current, your trace is not 24mils (0.61mm) passing across the hole. This is a custom PCB, not one of those cheapo Veroboards. It's actually about 3.81mm (150mils). You need to consider that if your PCB is the standard 1.6mm thickness, and the hole is through plated, the hole has tinning on it's cylindrical perimeter. Like so:-

thru hole

The implication is that whatever your actual trace width is approaching the hole, even if it was a micron and the annular width was a micron, you'd still have 3.2mm of copper along /across the depth of the hole. So it doesn't really matter if the hole is filled or not. It's actually one of the highest current capacity parts of your copper layer unless you have something > 126mils wide.


As mentioned earlier, use Ground planes. In Eagle, draw a polygon around the entire board and Name it Gnd. Do that for both the Top and Bottom layers. Rip up any Gnd traces you have. Add Vias in spots around the board and Name them Gnd as well to connect the top & bottom Ground layers.

On a 2 layer board, creating a Vcc (5V, or 3.3V)) is harder, those are usually routed as traces.


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.