6
\$\begingroup\$

I am working on a 4-layer board which integrates three 48 MHz ARM microcontrollers and a "Bluetooth module," along with some other features and supporting parts which are not so relevant to this question.

My stackup is as follows:

  • signals and most pads
  • GND
  • power
  • signals and a few pads

My GND plane is solid but I have split up the power plane to provide 3.3V local power nets for some of the ICs. Each of the 3 MCUs has its own Vdd area underneath, as well as an AVdd area fed from the local Vcc through a ferrite bead (as per the datasheet of the MCU). The BT module has its own digital Vdd. Differential stereo audio signals leave the BT module and are amplified into single-ended signals for output (to a car's audio system). This amplifier has its own local power pour underneath it.

Each of the local 3.3V nets is connected by a 10 uH inductor to the "main" 3.3V net, which contains a linear regulator. This is what the datasheet for the MCUs says to do, but I have applied it to the bluetooth module and the analog amplifier stuff as well. Each local net has a 47 uF bulk bypass cap, along with sufficiently many 100 nF bypass caps near the IC power pins. The datasheet for the MCU also calls for 10 uF caps, so I have included those as well. Would this application of the split power plane, inductor, and bulk cap be considered a best-practices approach to containing switching noise of the MCUs?

No traces cross the power plane gaps on the bottom layer, but many do cross on the top, the fastest of which carry signals which may switch at 2 MHz. My understanding is that the return current of traces running on the top will flow on the GND plane, which is solid. My conclusion is that crossing the power splits on the top is okay, but my knowledge of EMC is patchy, and so I am not 100% sure; there always seems to be something of which I am unaware. Am I correct in this regard?

Here's a screenshot of KiCAD showing part of the power plane: split power plane

Addendum: Like I said in the original post, traces on the back layer, which is adjacent to the split power plane, never cross gaps in the power plane, but many traces on the front do, as shown below (power pours are colored pink, traces are colored red, and the GND plane is colored yellow): crossing split power plane on non-adjacent side running parallel to split power plane on non-adjacent side

\$\endgroup\$
  • \$\begingroup\$ How good are you at keeping traces away from plane splits? \$\endgroup\$ – ThreePhaseEel Aug 3 '16 at 1:05
  • \$\begingroup\$ On the back layer, which is adjacent to the split power plane, I have kept every trace at least 24 mils away from the split, and of course, traces never cross the split on the back. On the front, there are a lot of places where traces cross or run parallel to and above the split between the planes. I will update my original post with a picture of how traces on the front cross the splits. \$\endgroup\$ – Zane Kaminski Aug 3 '16 at 2:47
  • 1
    \$\begingroup\$ There's a handy article on this by Henry Ott here hottconsultants.com/pdf_files/june2001pcd_mixedsignal.pdf I would also recommend his book Electromagnetic Compatibility Engineering \$\endgroup\$ – stefandz Aug 3 '16 at 6:50
  • \$\begingroup\$ I'm familiar with Ott's articles and was planning to read his book. Actually I haven't seen that particular article by him, but I've heard his explanations before; he is always quite convincing in his reasonings. Unfortunately, the article doesn't say much about splitting the power plane, other than that it's okay to do so long as you don't run traces across the split. I was hoping for something that went into a bit more detail about splitting the power up as I have did. I guess the takeaway is that my design is correct in this regard, but I was hoping for some more assurance. \$\endgroup\$ – Zane Kaminski Aug 3 '16 at 14:24
  • \$\begingroup\$ Your design does cross traces across splits though - my understanding is that this is non ideal. \$\endgroup\$ – stefandz Aug 3 '16 at 20:05
1
\$\begingroup\$

Your layout looks fine. At 2 MHz, there shouldn't be much to worry about. My only suggestion, if you haven't already, is to prioritize your most critical signals (probably analog and I2C/SPI) for your top ground coupled layer.

At higher frequencies (this includes critical fast slew rates), this topology would not be ideal. In that case we would remove the local power islands and if not possible, AC couple them with 100 nF caps.

\$\endgroup\$

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.