next topic »

[on:]

Hello

Decided to leave the (questionable) safety net of the auto router in Eagle and think a little more about my board layouts. First up are ground planes.

If I have ground traces on both layers of a two layer board should I have a ground plane on both sides or will one on the bottom layer suffice?

Is it advisable to create a "supply" layer in a similar fashion or is it sufficient to just make the supply traces thicker which is what I've seen people do.

My circuits are various Arduino based things working with MIDI and LEDs and button matrices, so lots of ATMega's and shift registers and what not.

Thanks
Jim

[Reply #1 on:]

The nice thing about having ground and supply planes on opposite sides of the board, other than the ease of routing, is that they form a nice big decoupling cap that smooths out your power supply.

[Reply #2 on:]

The nice thing about having ground and supply planes on opposite sides of the board, other than the ease of routing, is that they form a nice big decoupling cap that smooths out your power supply.

No, its a fairly small capacitor, order of 1nF for an Arduino-sized board - the important feature is the low-inductance path to the real decoupling caps.  A standard 100nF or 220nF decoupler far exceeds the board capacitance!

The basic rule for decoupling is having a low-inductance path from the supply pins to the decoupling caps - lets imagine switching 100mA in 10ns - that's 10MA/s which is going to cause 0.3 volts across 30nH - roughly the inductance of one inch of PCB trace...  If the decoupling cap is that far from the chip and with only normal traces, its supply voltage will fall or rise 0.3V during the switching event depending on the sense.

A plane has a much lower inductance (wider traces are better, a plane being the ultimate).  So long as each chip has a decoupler right next to it one plane is plenty - having two planes means that the siteing of decouplers is less crucial and one cap can serve many chips.

In practice the planes are rather broken up on a 2 layer board so it may be better to have ground plane on both layers to provide a single plane with better continuity - the continuity also means that long signal lines always have an adjacent ground return path which keeps their inductance down too.  With 4 or 6 layers its simple to have continuous plane(s).