Is it okay to have a section of the ground plane connected to the rest of the ground plane through a thin trace as long it does not carry lots of current (.5 mA approximately)?

There is an example:

enter image description here

Does it have any bad effect I am not aware of?

  • \$\begingroup\$ It should not. That is a very low current to even bother. \$\endgroup\$ – 12Lappie Feb 2 '17 at 18:05
  • \$\begingroup\$ So it doesn't have any undesirable effect to have the ground plane "split" in half? \$\endgroup\$ – jagjordi Feb 2 '17 at 18:16
  • 1
    \$\begingroup\$ For low frequency, not super-sensitive analog stuff, the odd ground plane split is unlikely to cause any major issues. Ground plane splits are of bigger concern when you need them for shielding (low impedance = good shielding, thin traces ≠ low impedance). But unless you're operating at multiple MHz (or well up in the GHz really) or super low currents (think nA or pA) then I don't see any real issues. \$\endgroup\$ – Sam Feb 2 '17 at 18:34
  • \$\begingroup\$ If your only concern is DC current then no, it shouldn't matter. If you have high-frequency or transient signals that use that ground path, or high-gain or sensitive amplifiers in that section, then that skinny ground connection may be an issue. \$\endgroup\$ – Paul Elliott Feb 2 '17 at 18:34
  • \$\begingroup\$ A 10 mil 0.5oz trace 0.1" long has a resistance of about 10m ohm. At 0.5mA it would drop 50uV. In some circumstances that would be unacceptable (for example, it's about a 1°C shift on some thermocouples). \$\endgroup\$ – Spehro Pefhany Feb 2 '17 at 20:17

Here's some general advice which may or may not be applicable to your circuit.

  • Interference pickup. One of the functions of a ground plane is to shield interference from other parts of the circuit, and the outside world. If you have a really large piece of ground plane which is connected only through a small track like that, the big plane may act as an antenna an pick up interference which might disturb the operation of the op amp. I would not suspect this to be the case in your layout, though. enter image description here
  • Length to the capacitor. The point of having a local capacitor near a a chip (C2 in this case) is to absorb fast current spikes without being hindered by stray inductance. But what you need to take into account isn't just the length to Vcc, but the total loop length from the negative supply pin to the capacitor to Vcc. You may want to consider moving the capacitor to the bottom of the chip and move the chip up a bit. Probably not a problem in your case, but something to keep in mind.
  • Before worrying about small stretches of thin tracks, you may want to beef up those anemic Vcc tracks. You could easily double, or more, the track width of Vcc, across the whole board. Once again not necessarily a problem but good practice. After all, the small stretch of ground track you're pointing to would not contribute much to lowering the total series resistance.
  • Changes in ground fill properties, or changes made by a careless board house. You have routed a track through the gap, which is good. The ground plane pour would not have filled that gap as you can see between pins 3 and 4. But even if it did, but you later changed the ground plane isolation distance, it might have ended up breaking the connection. Likewise, a careless board house could trim away that track, assuming it was just unnecessary ground fill and it would be better for manufacturing tolerances to remove it. Such things have happened "in real life" and should be considered.
| improve this answer | |
  • \$\begingroup\$ Thanks for your advice @nitro2k01 , just a question: i understand that tracks between pins should be avoided, right? \$\endgroup\$ – jagjordi Feb 2 '17 at 22:07
  • \$\begingroup\$ @jagjordi Not really. Tracks between pins are often fine, and in some cases, like parallel RAM circuits on older computers, it's absolutely necessary to be able to route the board. None of what I said are hard no-nos. Rather, they are risks and considerations, that you need to think about when laying out the PCB. \$\endgroup\$ – nitro2k01 Feb 3 '17 at 4:48

If this is a one-off (or low quantity) PCB then do yourself a favour and make it double-sided with a decent ground plane on the underside. What favour are you doing to yourself - minimizing the risk of EMC problems and cross talk or interference in your analogue circuits with other parts of your circuit. At what cost? Maybe a few dollars per PCB - how much do you value your time?

If this is a design intended for a product to be sold then it's the same argument - make it double sided to minimize EMC problems. At what cost? Maybe a few cents per PCB.

Let me try and justify this a bit more - the dual op-amp you are using (LM4558) as a comparator is badly decoupled - you have C2 on the positive pin but what tortuous route does it take to the ground pin of the op-amp? When that op-amp switches (comparator action with hysteresis via the 1 Mohm) you could easily cause ground bounce and you get a niggly little problem that bugs you and bugs you and, you regret the day you didn't pay the extra for a double sided board.

| improve this answer | |
  • \$\begingroup\$ Thanks for your answer @Andy aka, actually this is not even going to be produced since it was just me trying to design a pcb in order to practice so your answer will really help me in future designs that are actually produced. \$\endgroup\$ – jagjordi Feb 2 '17 at 22:01

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.