1
\$\begingroup\$

to keep this brief I am designing some audio circuitry and also need to design the power supply. The barrel jack in the schematic below sees 18VAC and I am converting that to +/-15V DC rails.

Schematic

So to tackle this I have routed out part of the board in the hopes that I can control the flow of the ground current and voltage currents while isolating any noise that may come from the other circuitry. Also note that the panel the audio jacks connect too will be grounded.

I am concerned I have overlooked something and was wondering if anyone with practical experience could advise on some things I may have overlooked. Or even if any of this is necessary.

Layout

How do I use slots in a PCB design such as this?

\$\endgroup\$
  • \$\begingroup\$ Are those slots milled through the board? If so, they look a bit too long - it would be easy to accidentally snap off the end of the board, especially if it has heavy caps on it. Why not just put a break in the ground pour instead? \$\endgroup\$ – Jack B Oct 10 at 17:06
1
\$\begingroup\$

Don't separate planes unless you have a good reason to. Henry W Ott says there are very few reasons to do this.

The most important thing that I can say about slots in ground planes, is don't have them! If you do have slots, no traces can cross over them. If a trace does cross over the slot ask yourself this question: Where is the return path for the current? Remember the fundamental principal of EMC, "return currents locally and compactly, through the smallest loop area possible." If everyone would follow this principal, a great many of our EMC problem would go away or at least be minimized.

Source: http://www.hottconsultants.com/techtips/tips-slots.html

Separating planes is should be looked at as a way to reroute currents. There are consequences to this.

The first one is that it creates more resistance (and inductance) between the power source and the components.

The second one is it can create nice dipole antennas at higher frequencies and turn a product into an unintentional radiator.

The third problem is slots can reduce heat spreading capabilities of the internal plane (which could be good or bad, depending on your situation)

While this board is redirecting current through the slots, it is also creating resistance, the resistance can be calculated, and you could draw in two small resistors between the ground of the power section of the design and the rest of the board. These resistors will create common mode noise and voltage rise with large currents.

enter image description here

This slot might be useful as it blocks current from running under the potenitometer (if it has a ground connection) and keeps it away from the J8 connector. Which would be blocking currents that want to go straight back to the source.

enter image description here

It might be wise to consider opening up the slot between C118 and C116. I can also see no useful purpose for the slots around U18 and U17 unless the intention is preventing heat from traveling to the rest of the board.

Another thing: You also don't need slots cut into the PCB, if your intention is to route return currents then keep the PCB and add slots in the internal plane. PCB material is resistive. With that much of the PCB gone and heavy components such as large caps, I would be worried about the PCB failing mechanically with the amount of material present.

\$\endgroup\$
  • \$\begingroup\$ Great advice, thank you very much. Regarding U18 and U17, the slots are indeed there for heat to prevent the electrolytic caps from getting too warm. Your answer is great and has given me a good bit to think about. I will probably remove the slot between c116 and c118 as I feel it will rid of any resistance issues. I will keep the slot near the supply input to prevent return paths over the components. \$\endgroup\$ – Adam Oct 11 at 8:35
  • \$\begingroup\$ You could also remove the slots, and put slots in the ground plane, which would have a similar thermal result. If you like the answer, then upvote and mark the appropriate answer as answered \$\endgroup\$ – Voltage Spike Oct 11 at 17:46
0
\$\begingroup\$

Ask yourself where the current loops are...

The AC loop is clearly J10 -> diode -> C(116,121) depending on instantaneous polarity then back to the power jack. It is this loop that potentially causes you hum, or buzz problems, especially since the cap charging current pulses are large and harmonic rich.

Were I doing it I would :

  • Make an explicit connection between the caps and the AC input common that is entirely separate from your ground plane.
  • Connect the ground plane to the cap common point at ONE point to avoid cap charging current flowing in the plane.
  • Place an RC snubber across those diodes (Or pick Shockley instead of very slow SI junction parts with massive reverse recovery charge).
  • Only having done these things would I consider splitting the ground plane (NOT The whole board, that is painful mechanically), but note that you must never run any trace across a split in its reference plane. Howard Johnson gives good advice in 'advanced black magic'.
\$\endgroup\$
  • \$\begingroup\$ Great stuff so you are suggesting to have a separate ground trace for all of the caps and power electronics first, in isolation to the ac input. Then seeing if it is necessary to split the ground plane. Also I will definitely put the RC snubber in! \$\endgroup\$ – Adam Oct 11 at 8:53
  • \$\begingroup\$ Also, might I ask, how would I calculate the RC snubber value? \$\endgroup\$ – Adam Oct 11 at 9:00

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.