Comments on 4-Layer PCB Routing Question
Parent
4-Layer PCB Routing Question
I am designing a 4-layer PCB that has both analog and digital circuitry throughout it. The analog section involves high return currents as well as ADCs sampling the voltage across sense resistors among other things. The digital side does not have high-frequency communications - PWM at 25kHz, and a Two-Wire bus at a couple of hundreds of kHzs.
Here is my stackup:
1 - Signal
2 - GND
3 - PWR
4 - Signal
What is best practice when routing a design like this? Right now I am routing traces from both the analog and digital components on the top layer and moving to the bottom only when I run out of room. Is this correct, or should I use the top layer for analog only and the bottom for digital only, or vice versa?
Post
1 - Signal
2 - GND
3 - PWR
4 - Signal
This seems to be common advice, especially on the 'net someplace, but that doesn't make it good.
Stop and actually think about what problem you are trying to solve with each layer. What exactly do you think dedicating a whole plane to just power will do for you? Unless this is a exceptionally high current design (and then there are other solutions like bus bars), I can't even guess why you think layer 3 makes any sense.
What you should do:
- The top layer should be used for interconnects as much as reasonably possible. This is the one layer the parts are connected to already, so makes the most sense to use as connections between parts.
- The next layer down should normally be a ground plane, if you have routing space for that. This is the layer closest to most of the signals, so makes the most sense for a ground plane. High frequency return currents in the ground plane will follow underneath the outgoing currents. Having the ground plane close to those outgoing currents reduces the vertical component of the loop area.
The ground plane also act like a shield. Since most signals are on plane 1, plane 2 is the most effective place to shield those plane 1 signal from those on other planes. This is also a good argument for routing the sensitive signals on plane 1 first. That way they are better protected from signals on planes 3 and 4.
- When you can't route signals on plane 1, use plane 4 next. This is the plane easiest to make changes to by hand. Every design starts with the first board, and those sometimes need changes. Keeping signals on outer planes makes those changes easier.
- Use plane 3 last. Use it only when you need a third plane to make connections. This happens most under dense parts, like microcontrollers.
- Carefully bypass the power feeds to each part, and keep the high frequency currents thru those parts local. The connections from power lead to bypass cap, to ground lead should be as short as reasonably possible, and should NOT cross the main ground plane. If you run these high frequency currents across the ground plane, then you don't have a ground plane anymore, but a center-fed patch antenna.
Connect the ground of each part to the ground plane separately, with a single via close to the ground pin. The high frequency currents produced by the part are shunted by the bypass cap and don't run across the ground plane. The ground feed therefore sees reasonably well-behaved currents that don't cause much trouble to the rest of the circuit.
Note that by following the decoupling rules above, all power feeds are low impedance at high frequencies at each point of use due to the bypass caps. Since low impedance at high frequencies is handled locally, the power feed only needs low impedance at low frequencies. Average copper traces have plenty low enough resistance for most ordinary applications. A few mV of drop between the voltage regulator and the point of use is usually not an issue. If the power currents are high enough, then you can make the power traces wider. That still doesn't mean they need to be whole planes.
0 comment threads