# Details on PCB layout for microcontroller

Update: the follow-up question shows my take on the resulting PCB layout.

I'm laying out my first board with a uC (I've got a reasonable amount of experience in using and programming embedded systems, but this is the first time I'm doing the PCB layout), an STM32F103, this will be a mixed-signal board using both the internal DACs of the STM and some external DACs via SPI, and I'm a bit confused about the grounding.

clearly state that I should have a local ground plane for the uC, connected to the global ground at exactly one point, and a local power net, connected to the global power near that same point. So this is what I'm doing. My 4 layer stack is then:

• local GND plane + signals, uC, it's 100nF decoupling caps, and the crystal
• global GND, unbroken except for vias. In accordance to sources such as Henry Ott, the ground plane is unsplit, with the digital and analog sections physically separated.
• power, a 3.3V plane under the IC, thick traces for the 3.3V external DACs, thicker traces for distributing the $\pm15$ volts in the analog section.
• signal + 1uF decoupling caps

Further away on the board the analog components and signals are on the top and bottom layers.

So the questions:

1. should I break the global ground under the uC, or is it good to have the full ground plane under the local one?
2. Power plane: I'm intending to have a power plane only under the uC and use vias to bring the power to the decoupling caps and therefore the uC on the top layer, as I can't really use one much elsewhere. The external DAC's should be star distributed, so I have separate tracks for them, and the rest of the board is $\pm15$ volts. Does this sound ok?
3. I'm using both the ADC and DAC of the uC, and generating a reference voltage in the analog section of the board, which I bring to the Vref+ pin of the uC with a track on the power plane. Where should I connect the Vref- pin: local ground, global ground, or make a separate track on the power plane connecting it to the global ground in the analog section, where the ground should be quiet? Maybe near to where the reference voltage is generated? Note that on the STM32 the Vref- is distinct from the analog ground VSSA pin (which I suppose goes to the local GND plane?).

Any other comments on the design here are of course welcome too!

• A lot of searching questions resulting in a lot of good answers with good comments. However a lot of what is good practice can be learnt by studying what others have done. Take a lot of good quality (similar 4 layer) mixed signal PCBs and use a hor air tool to desolder large components. Investigate how the power vias are managed. You want to learn the best practice from professional designers as some of the stuff never gets into books, it is just in house rules of thumb, transmitted by oral and (over shoulder) proximity tradition. Do not pay as much attention to cheap consumer designs. Apr 28, 2016 at 20:50

You don't necessarily need a local ground plane for the micro. The local ground can be a star with the central point under the micro, which is where this star is connected back to the main ground, for example.

If you have at least 4 layers, then it can make sense to dedicate one of the layers in the immediate vicinity of the micro to a local ground. If this makes routing too hard or this is a two layer board, just use the star configuration. The main point is to keep the high frequency power current drawn by the micro off the main ground plane. If you don't do that, you have a center-fed patch antenna instead of a ground plane.

The loop from micro power pin, to bypass cap, to micro ground pin should not cross the main ground plane. This is where the high frequency power currents will run. Connect the ground pin to the main ground in one place, but do not connect the ground side of the bypass cap to the main ground separately. The ground side of the bypass cap should have its own connection back to the micro's ground pin.

Digital signals going between the micro and other parts of the board will still have small loop area because the micro will be connected to the main ground close to its ground pin.

• Olin, if you could post some references to back your "patch antenna" theory, that would be appreciated. Jan 9, 2016 at 18:14
• @Timo: The Vref- pin draws very little current, and is used as the 0 reference for the A/D. This should be connected straight to the main ground plane with its own private via. Jan 9, 2016 at 22:01
• @Arm: I'm not saying the ground plane shouldn't be solid. It's the way the processor's ground is connected to it that matters. Look closely, and you may see a local ground net with a single connection to the main ground. Also, a lot of times you can get away with less than best practises. Open source projects don't have to worry about the cost of field failures or that 1 in 10000 case where it doesn't work quite right, or even a lot of times about emission limits (not that it's legal, but much less likely the FCC is going to notice). Jan 9, 2016 at 23:16
• The issue with the Vref+ pin is that you want to keep noise off of it. You're not worried about it polluting the rest of the system. If you're using it, it's probably coming from a separate regulator anyway. You can connect the other side of its bypass cap to the main ground, or connect it to the analog ground pin if this chip has one, then connect that net to the main ground near the analog ground pin. Jan 10, 2016 at 14:08
• @Bip: Again, the local ground isn't necessarily a plane. Jan 13, 2016 at 15:17
1. No, you should not. And get rid of the so called "local ground". What do you think is happening with all the digital signals when you implement this local ground? You should find the answer in Henry Ott's article that you linked, Figure 1.

Sure, you do have a connection between local ground and the ground plane, but all you do is increase the loop area, essentially turning your trances into small antennae.

2. That sounds fine.

3. The reference manual says that VREF- must be connected to VSSA which in turn must be connected to VSS. I suggest that you just connect the VREF- directly to ground and try to keep digital currents out of the way using clever placement.

As for the suggestions, if 1uF caps are the only components you plan to place on the bottom, I recommend that you place them on top. When you have components on both sides, the manufacturer either has to run the board through the oven twice, or solder the components by hand. Both of which will increase the manufacturing cost.

• You may want to include a link to the Ott article you're referencing. Jan 9, 2016 at 17:50
• @akohlsmith I was referring to the same article as OP, but added a link now. Jan 9, 2016 at 17:53
• There's quite a lot of components on the bottom in the analog section, so it's not just the big decoupling caps.
– Timo
Jan 9, 2016 at 19:33
• Sorry, I would have really wanted to accept half of your answer and half of Olin's if that were possible, but decided to go with Olin's since the local ground plane is what I ended up doing (as seen in the other question)
– Timo
Jan 12, 2016 at 11:39

You may find this answer useful.

There are a very few times I use truly separate planes (such applications still exist), but not for a circuit such as yours.

Careful placement of components and a bit of thought on the power / ground should help you achieve a good layout.