Two questions on beginner PCB design:

  1. For integrated chips on PCB design, can you draw routes from the side of the contact pad, or is it standard practice to go head-on straight to the pad entry?

    Two Options to Access Routes to a IC

  2. For large capacitors that have an output to GND, on a board that has a GND plane, can you put a via directly to the GND plane? Does this help dissipate heat?

    Location of Potential Vias on GND of Capacitor

  • \$\begingroup\$ The answers give you a start with 2., also see What is the difference between "via-in-pad" and a via in a pad?. Nick's answer there is quite informative on how these are constructed. \$\endgroup\$
    – Mast
    Nov 29, 2023 at 8:53
  • \$\begingroup\$ For the via in pad it is custom to place it at the side of the pad, not in the middle of it. Otherwise it may affect the wetting when the component is soldered. Also if the via is attached to a ground plane, it should not get directly attached to the pad but placed at the side of the component with thermal relief traces in between - otherwise the layout may affect soldering of the component. \$\endgroup\$
    – Lundin
    Nov 29, 2023 at 9:45
  • \$\begingroup\$ Note that the via-in-pad stuff is about manufacturability (i.e. low defect rate) using reflow soldering. If you're a hobbyist soldering one board by hand, it's not really something you have to worry about as long as the vias are small; you'll be watching all of joints as they form and can add more solder if you need it. That being said, you shouldn’t need to put a via in the pad. Small (ceramic?) capacitors shouldn’t heat up much. If they do, I recommend adding copper around the pad instead of messing with vias. \$\endgroup\$
    – Adam Haun
    Nov 29, 2023 at 17:25

3 Answers 3

  1. You can route your signals to whatever point of the pad that is convenient for you, it does not matter (at least not until you go into very high frequencies). So both options on your image are equally valid (you can even connect with a diagonal line, or on the "inside" side).

  2. What you are drawing on your second image is called a "via in pad": it is perfectly allowed, but requires the via to be filled (epoxy or metal) before soldering the capacitor (otherwise the solder paste will flow into the via, with a great risk of getting a bad solder joint). Most PCB manufacturers can do via in pad. But usually, they charge extra for it (so if you can avoid using via in pad for your design, it's cheaper).

For thermal dissipation, all depends from where to where you want to dissipate heat (from the capacitor itself to the ground plane?). Often, the best solution if you can, is to add a ground "plane" as big as you can on the top layer. If you need additional transfer to ground plane on an internal/bottom ground plane, then add as many vias as you can (if heat comes from the capacitor, one via beneath the capacitor is probably slightly better than one next to it, but vias all around would be even better is you have enough space.


For (1), yes, you can certainly do that. The only case where it might be a problem is when it's a very high-bandwidth controlled-impedance signal, but if it's a high-bandwidth controlled-impedance signal it's not going to be on the edge of a chip anyway.

For (2), this can cause manufacturability issues. I recommend you look up the term "via-in-pad" for more information; in short, the via can wick away solder during reflow, leading to a poor solder joint. There are ways to get around this when you need a via in a pad, but they add a lot to the cost of the board.

Also, if you are having thermal issues with a capacitor to the point that you need to consider heatsinking it, you're almost certainly doing something very wrong.

  1. Yes, though I would avoid going directly between two adjacent pads if they are very close. This looks like a short-circuit when soldered, making it harder to spot any real short-circuits.

  2. If the pad is large compared to the hole, via in pad area is fine even without filled vias. My own rule-of-thumb is that filling is needed if hole diameter is more than 10 % of pad size. For example, a 3x3 mm pad with 0.3 mm via is fine, the amount of solder that may wick into the hole is insignificant.

  • \$\begingroup\$ I would call that 1% of the pad size (by area) \$\endgroup\$ Nov 29, 2023 at 12:04
  • \$\begingroup\$ @JasenСлаваУкраїні Yeah, though I find it easier to think by sizes. And in a long narrow pad, you don't want a wide hole even though the pad area would be large. \$\endgroup\$
    – jpa
    Nov 29, 2023 at 12:07
  • \$\begingroup\$ Huh... are there really that many situations where you've got a giant pad but no room to escape it? \$\endgroup\$
    – Sneftel
    Nov 29, 2023 at 13:57
  • 1
    \$\begingroup\$ @Sneftel Usually only in double-side assembly where the other side layout limits where you can put vias. Vias in large pads can also be useful for mechanical stability and heat transfer, as implied in question (even though capacitors rarely need cooling, transistors and chips do). \$\endgroup\$
    – jpa
    Nov 29, 2023 at 15:02

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.