1
\$\begingroup\$

I have designed my first pcb (4 layer) and I have a question about power planes versus power traces. I am using KiCad 7. I have tested the circuitry on a proto-board.

I have a high current section (12-15 V dc @ 3-6 A for 100 - 500 msec), and a lower powerlogic control section (3.3V) - a DAC and ADC controlled by a Raspberry Pi SPI buss (2.4 MHz). I have 2 signal layers, front and back, a ground plane, and a power plane (green). I am debating whether I should (1) use a power plane for the logic chips or just larger traces, and (2) whether I should use a couple of power planes for the high current section or just really fat (5-7 mm) traces.

I have attached two pictures that show the power layer traces in green and potential power planes. Creating a power plane for the logic portion of the design seems to be a good idea. However, the high current section is broken up into so many pieces (e.g. power connector, then a fuse, then a switch, then a relay etc.) that perhaps the fat traces are a better design. What do you think?

enter image description here enter image description here

\$\endgroup\$
3
  • \$\begingroup\$ Planes give power resistance, but as long as the resistance is acceptable, you could use either. However one thing that jumps out at me is the large number of huge through hole resistors you're using. That board would be a lot smaller and the layout much better if you used modern SMD resistors. This would also make it much easier to have the board manufactured as well if you eventually choose to do that. \$\endgroup\$ Commented Oct 27, 2023 at 18:45
  • \$\begingroup\$ I agree with your comment regarding SMD parts. I don't have a way to solder them, so I went old school. On my next board, I will use them and other SMD parts. I was really looking for a recommendation - use the ground plane or not. \$\endgroup\$ Commented Oct 27, 2023 at 21:13
  • \$\begingroup\$ If you're assembling these by hand, you can generally use the same tools for SMD and through hole parts, although you may want to buy a finer tip for your iron. \$\endgroup\$ Commented Oct 28, 2023 at 0:10

2 Answers 2

1
\$\begingroup\$

There are several reasons to switch from traces to planes:

  1. The current is so large that the traces may heat and cause the board or components to thermally fail.
  2. You have multiple components using the same net, and it's hard to route a trace to all of them. This is very common for ground.
  3. You have a few components that are very hot, and you want to pull heat way from them.
  4. The current is so large that the voltage drop across the trace is unacceptable.

7 mm wide traces will work for 6 A, so #1 isn't a concern IPC-2152: Standard for Determining Current Carrying Capacity in Printed Board Design

enter image description here

You were able to route without the plane, so #2 isn't a concern. Without knowing the application, it's hard to say if #3 or #4 is a concern, but the meandering ground trace seems worrisome to me. Do to the high current, you might have voltage drops along your ground trace. It might we worth adding a ground plane so that ground potential doesn't change along the trace.

The other thing that seems troubling is traces are running parallel to each other for long stretches without returns next to them. You may have cross talk issues with your high speed traces. Adding a ground plane under and between traces provides a return path for signals to reduce cross talk. Rick Hartley gives an excellent talk on this How to Achieve Proper Grounding - Rick Hartley with the pertinent portions being from 10:20 to 1:04:00. The short version is:

  • All signals need a return path.
  • If you don't provide good return path (such as a ground plane), the signal might return along a path you don't want (say another trace) which causes cross talk.

At the very least, flood all open space with a ground, and stitch the planes together with vias.

\$\endgroup\$
1
  • \$\begingroup\$ I have signals (red/orange) running on top and bottom, a ground plane (blue) on one inner layer, and power on the other inner layer. I am mostly worried about #4 in your list. I had some issues in my bread board setup with voltage sagging when I was running at full power. BTW, the application is igniting model rocket motors. Based on your pictures, are multiple planes with small gaps between them a better solution than fat traces? \$\endgroup\$ Commented Oct 27, 2023 at 22:28
1
\$\begingroup\$
  • If it is possible, you can have Power track repeating on multiple/all layers and stitch them together with vias, this helps.
  • Increasing PCB copper thickness from 35 micro to 60/70 micro will help but increase cost, see if that could be a solution
  • you can remove green mask on the track that will allow putting solder to increase thickness of the track.
  • please use PCB layout guidelines define in device manufacturers datasheet, for power devices most of the time they provide ref layout also.

Some pictures to help understand better.

PCB with removed solder mask
Figure 1. PCB with removed solder mask
from EE.SE question "Fortifying PCB traces with solder?" by ElectronSurf

Power traces/polygons with Vias
Figure 2. Power traces/polygons with Vias
from Monolithic Power Systems - Motor Driver PCB Layout Guidelines – Part 1

USB PD Power track with Vias
Figure 3. USB PD Power track with Vias
from my personal PCB design

I hope this helps

\$\endgroup\$
1
  • \$\begingroup\$ Great references! Thanks! How much space do you leave between the power planes? \$\endgroup\$ Commented Oct 30, 2023 at 14:41

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.