PCB 6-layer stackup problem

Question

I'm currently designing a PCB with double side components and I'm limited to 6 layers max. The project has couple of MCUs at 84 MHz. There are USART, I2C, SPI, some analogue lines and high-power lines in the design but not any high-speed lines. There are also some very short RF lines for antennas.

The problem is due to the high density and limited size of the PCB I can't use this stackup: S-G-S-S-P-S At some parts of the PCB specially around the high pin count MCUs there's need for signal lines to go through the ground or power plane.

Also all the power electronics and switching components are on the back side.

This is the stackup properties provided by the PCB manufacturer:

So my main concern is if routing some signal lines through the power/ground plane will cause me problems or not?

Answer 1

3 basic rules

Rule #1: Bandwidth is not the clock speed rather the rise time f-3dB=0.35/Tr (10~90%) so you probably want thinner dielectric than normal for lower impedance tracks

• this helps keep track/gap <= 5 mil (127 um) and < matched via impedance which raises L but thinner dielectrics raises C to maintain Z^2=L/C Also 3 mil (64um) track/gap is doable by good shops.

Rule #2 avoid crosstalk with adjacent SS layer parallel tracks.

Rule #3: Use lots of microvias for PS layer connections to other layers grids and appropriate decoupling cap per IC. If a Microvia is 50 Ohms on a power supply that is 50 mOhms, how many do you need? ( not depends on decoupling caps and rise time and ringing tolerance)

If you don't already have , get Saturn PCB Design Toolkit

Answer 2

Experienced PCB designers DO NOT route signals on power and ground layers all the time. They just don't do it unless there are no other ways to complete the routing.

You might need a lot of vias to complete your routing.

Reduce the size of your vias.

In high density boards I used the following via:

copper pads on top = 0.45 mm
drill = 0.15 mm
copper pads in inner layers = 0.45 (*)
copper pads on bottom = 0.45 mm

(*) Whenever I can, I enlarge inner pads 0.55 mm to make the PCB manufacture happy.

There's no extra cost to pay for these vias. They fit their standard manufacturing flow.