I have a 2 layer PCB. Bottom layer is ground plane (blue in images below), top layer is power and signal traces and the rest is ground pour (red in pictures below). Vias are connecting the bottom and top ground layers.

I am using fusion 360 for designing my PCBs and the copper pours fill whatever void the traces leave behind. I am wondering however if the filling obtained this way is optimal.

Consider the two pictures below, the difference is that on the right picture the copper pour extends a bit more, on the picture to the left I have prevented it from doing so because I did not see the point of having it extend like that, that is where it does not connect to any ground pin of any component.

Should I do that or not ?

enter image description here

  • 1
    \$\begingroup\$ There's no right or wrong here, do as you like. \$\endgroup\$
    – MiNiMe
    Commented Sep 19, 2023 at 21:07
  • 1
    \$\begingroup\$ ...Oh, there are actually stitching vias in there! I had to look at that for some minutes before realizing. In the future, please use better contrasting colors to make these more obvious. \$\endgroup\$ Commented Sep 19, 2023 at 22:29

1 Answer 1


Understand that, since a schematic isn't given, we cannot comment on what the circuit is doing, and how suitable the layout is for that purpose.

Regarding the highlighted area, probably not much, if anything. I would prefer the right side, for two reasons:

  1. More copper means more thermal conductivity, even if the immediate/overlying component can't make direct use of it (compare the others with thermal pads).
  2. Stitching vias can be added to the peninsulas, further reducing ground impedance in the local area.

There is an even better improvement: the diagonal -12V_LOC trace can be jogged out around the BOTT_LT45_SET_OUT polygon, allowing top GND to pour around the latter, connecting directly to the nearby -- bypass capacitors? -- without vias required (but the vias can be kept anyway for better stitching).

Oddity: top and bottom side thermal relief differ on thru-holes. This doesn't do anything, it's just... odd.

Speaking of thermals, you aren't making great use of the thermal pads on applicable devices: U? (er, do any chips have designators on this? at all? odd..), well the one beside R23 anyway, appears to have GND, but it's narrow spoked to surrounding metal, and has no vias. It's safe to put several vias (for something this size, 4 to 8, of ID 0.2-0.3mm) inside the pad; on typical processes, untented vias of this size wick very little solder, or indeed it may be advantageous to wick some excess solder to prevent the device floating up and potentially having poor connections to the pads. (This is a leaded (MSOP?) device I think, which generally doesn't quite fit flat, i.e. the leads sit very slightly proud of the under-pad plane, and extra solder may be desirable to reach that, after all; the above is most relevant to SON/QFN where the leads and middle pad are coplanar.) In any case, the thermal relief can be disabled for this pad (or fixed fill added on top), and vias added flanking the pad if nothing else (which then can be tented).

Hm, there's also missing copper under the, R23 label, and some trace hooking around but doesn't seem to connect to anything..? Not sure what's going on there. Generally prefer solid ground pour under everything. (You've done this pretty well overall, I think, with the +12V_LOC jumper top-right being the longest visible here.)

Finally, layout could be slightly improved by the +12V_LOC trace. This is the longest bottom-side trace visible, but the reason is understandable: alternative routes are generally even less appealing, under C9/R10/EPAD for example would cut right through both top and bottom GNDs, making things much poorer overall. That said, consider the vertical segment right of R10: this could be nudged to the right, so that the top side peninsula near the EPAD, and immediately beside R10, can be stitched to bottom GND right there. Probably just bump over that one row of stitching vias. Likewise, push out the diagonal corner piece, so that the 45° peninsula top-right of C8 can stitch to the same bottom GND. Alternately, or additionally, the bottom trace could be jumpered to the top briefly, in either otherwise-open patch of GND, so that bottom GND can flow through this area; that is, make it as a short bottom-side jumper to cross the BOTT_A_IN- trace, come back to the top and move over a bit, then jumper under the BOTT_A_OUT trace (and maybe -12V_LOC too; or even short-jumper under all three). In any case, this helps support low impedances / high frequencies on the BOTT_A_IN- and BOTT_A_OUT traces going up and right, keeping ground contiguous underneath them, or ground very near them while having the least loop perimeter of the ground void they're crossing.

Again, to reiterate, no idea how relevant these steps are to the immediate design, if they are at all. The above are general changes that I would make in my own designs, regardless of nature; if nothing else, as an exercise to better hone my intuition over routing and grounding.

I gather this is an analog board, amplifier or something, so high frequencies are probably not important, functionally speaking. Still, poor routing and layout around connectors and cables can invite RFI into the system; perhaps ferrite beads and small bypass caps should be considered on some signal connectors? If it is actually a switching supply, or class D amp, or digital or networking device or whatever, pay attention to edge rate, as it's what matters, not the clock speed -- the peak transient from a clock edge doesn't care how often it's excited, it's there even from just one.

  • \$\begingroup\$ Thanks for the answer, I am actually a beginner hobbyist, so some details of your answer I do not understand yet, but I will try to understand and implement the changes you mention \$\endgroup\$
    – DarkBulle
    Commented Sep 20, 2023 at 0:05
  • \$\begingroup\$ The hooking trace connects to the bottom right pin of the IC \$\endgroup\$
    – DarkBulle
    Commented Sep 20, 2023 at 0:10
  • \$\begingroup\$ On the top yes, but the bottom seems to mirror it for no reason; it's not clear what it connects to from this view. \$\endgroup\$ Commented Sep 20, 2023 at 0:11

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.