GND routing, they choose the long way even with a gndplane near: why?

[mcinque]

I was replacing the transistor who drives a magnetic buzzer on this RC battery charger, and noticed that the engineer who designed it, has chosen to route the emitter as close as possible to the 7805 ground pin, even with a ground plane near.

The transistor current drain is very small I guess, so I think that no issues (like ground bounce) can occour routing the emitter to the near groundplane, but since I've a lot to learn I'd like to have some suggestions by you: is this is a required routing or it's over engineered?

[Tandy]

Auto router?

[nctnico]

I think they didn't want the current from the buzzer through the ground plane. Also note how the plus and return of the buzzer are routed parallel to minimize the loop area. Perhaps the buzzer has some EMC issues when there is a large loop.

[SeanB]

It is a little anal, but they can be absolutely sure they have no problems then, plus if they need to drop the volume they have a easy to cut trace to add a bodge resistor. Note as well the 5V rail is also supplying the connector and some unpopulated pull up resistors as well, and there is a small ceramic decoupling capacitor there as well returned direct to the ground plane.

[ajb]

You said it's a battery charger, so it's bound to have some fairly critical voltage and current measurement happening. The current measurement in particular could involve substantial amplification to allow the user of a low value measurement shunt, so you'd need to be particularly careful about running large currents around the current sense amp, as even a small error term there could be amplified into a much larger error in your measurement.  Then, if you're using a ground-referenced single-ended ADC to digitize the current and voltage measurements you need to be sure that your "ground" reference is the same between where the signal is generated and where it's measured.  So you need to avoid running large currents through the ground plane in a way that would introduce a voltage gradient between those two points.

Of course whether or not the design is sensitive enough that running that speaker through the ground plane would have caused a problem is impossible to say without a more detailed analysis.  But it looks like the designer didn't have to go to much trouble to isolate the speaker current, so if nothing else it was cheap insurance, and good defensive design.

[AndyC_772]

It may simply be a mistake by the designer. The lowest resistance, lowest inductance path between two points is almost always through a plane, and by routing a separate trace, the designer has added both, as well as constructing a radio antenna that didn't need to be there.

Although routing like this is often done deliberately and with the best intentions, it's also often misguided and actually worse than simply joining everything that's meant to be grounded straight to the GND plane.

[georges80]

As per AJB's post, it is most likely to not have ground currents/noise flow through that area of the ground plane. It is essentially a star routing scheme where the buzzer ground has been returned close to the regulator. The design was either being cautious or on an earlier rev they found problems. It's definitely not an autorouter issue - that's a hand routed board - I rarely find a PCB layout engineer that bothers to use an autorouter.

I've had to do similar cuts in ground planes where high switcher ground currents can cause enough ground bounce in a uC to brown it out. It is often NOT a good idea to tie everything to a large ground plane especially in mixed signal circuitry. Where bypass caps get their ground can affect their 'positive' end due to ground bounce effects.

Understanding the ground currents and how they can cause ground bounce in various circuitry is critical to a reliable pcb layout implementation. Especially where you may have several voltage rails/regulators and a single ground reference net.

Just by having a large single ground plane does not guarantee that the voltage at one end/location of that plane is instantaneously the same at another end/location, especially in a 2 layer board where the ground plane (not really a plane, just flooded copper) gets cut in a lot of places and currents flow differently in the remaining paths.

cheers,
george.

[T3sl4co1l]

Looks like misplaced caution.

If you aren't absolutely sure what you're doing, a ground plane for all nodes is almost always better than trying to hack it otherwise.

Yes, routing those traces together will tend to reduce EMI, but has that principle been applied consistently?  One tiny buzzer at 2kHz seems a preposterously low priority considering the likely noisy digital logic sprawled out elsewhere.

Consistency is another one of those things that bugs me.  Lots of average designs are inconsistent, sloppy, careless.

Using such examples as reference obviously doesn't make for good learning opportunities..

The entry angle of the trace into the plane seems to suggest it was routed before pouring, and the pour was made later as an afterthought.  Possible it was even a revision hack, done in the laziest way possible.

There are no thermals on the pour, and the pour is bottom side only.  This is bad for fabrication because the copper imbalance causes the board to warp slightly.  Maybe not a big deal for QFPs, but a possible problem for QFNs, LGAs, CSPs, etc.  Lack of thermals won't matter much for an apparently wave soldered board, but does seem to show lack of consideration.

Tim

[mcinque]

Thank you all for your kindly and technical replies. I really appreciate your teachings and thoughts. I've a lot to learn but luckily you've a lot to teach me

Thank you